A collection of libraries and tools that let the user handle OpenFOAM-data based on expressions
This file gives an overview of swak4Foam and a history of the
features. It is not a canonical documentation.
This file is written in the mighty org-mode (see
http://orgmode.org/) a markup/outline-mode for (X)Emacs. Using this
mode it can be easily (using 3 keystrokes … it’s Emacs) to PDF or
HTML to make it more readable (and add a table of contents).
Please don’t try to “beautify” it with any other text editor as
this will surly mess up the markup (and keeping the file
org-compatible outside of the org-mode is a pain in the neck.
The Markdown-variant README.md is only there to be displayed in a
human-readable form by the web-interface to mercurial at
sourceforge.net. It is generated from REAME and only updated
during releases. Don’t edit it.
Bernhard Gschaider (bgschaid@hfd-research.com)
Bernhard Gschaider (bgschaid@hfd-research.com)
In alphabetical order of the surname
- Martin Beaudoin
trackDictionaryinsimpleFunctionObjects- Martin Becker
- The
potentialPitzDaily-case (demonstrating a problem withgroovyBC) - Oliver Borm
patchMassFlowAverageinsimpleFunctionObjects- Peter Keller
sprinklerInlet-case- Martin Kroeger
mtvsurface writer insimpleFunctionObjects- Andreas Otto
- fixed the
circulatingSplash-case - Alexey Petrov
pythonFlu-integration- Bruno Santos
-
- Compilation with Intel compiler and Mingw
- Rewrite of
mybisonandmyflexto allow parallel compilation withWM_COMPPROCS - Generation of dependencies for files that need Bison generated tab.hh files. This allows not having race conditions during parallel compilation
- Hrvoje Jasak
- Fixes to compile on Intel and CLang
- E.David Huckaby
- Add the writing of particles to
writeFieldsOften - Alexey Matveichev
-
- release generation script.
- Automatic
swakConfiguration
- Mark Olesen
-
- port to OpenFOAM+ v1612
- improvements to scripts
- Philippose Rajan
-
- Bugfix for segmentation faults in parallel
If anyone is forgotten: let me know
According to the commits in the mercurial-repository (and
the repositories of the projects from which swak emerged)
contributors are (ordered by the year of their first contribution):
- 2006-2017 Bernhard F.W. Gschaider <bgschaid@hfd-research.com>
- 2008 Hannes Kroeger (hannes@kroegeronline.net)
- 2008-2009, 2012 Martin Beaudoin, Hydro-Quebec (beaudoin.martin@ireq.ca)
- 2010 Marianne Mataln <mmataln@ice-sf.at>
- 2010 Oliver Borm (oli.borm@web.de)
- 2011 Alexey Petrov <alexey.petrov.nnov@gmail.com>
- 2011 Petr Vita <petr.vita@unileoben.ac.at>
- 2012-2016 Bruno Santos <wyldckat@gmail.com>
- 2013 Georg Reiss <georg.reiss@ice-sf.at>
- 2014 Hrvoje Jasak <h.jasak@wikki.co.uk>
- 2014 David Huckaby <e.david.huckaby@netl.doe.gov>
- 2015 Domink Christ <d.christ@wikki.co.uk>
- 2015 Alexey Matveichev <alexey.matveichev@gmail.com>
- 2016-2017 Mark Olesen <mark@opencfd>
See: http://openfoamwiki.net/index.php/contrib/swak4Foam
- Version 2.0 or higher of OpenFOAM and version 3.0 or higher of
Foam. The
OpenFOAM-devis also supported but because this is frequently changing compilation may fail. The branchfeature/port_of-devof the development repository may work better - the compiler generators
bisonandflex- bison
swak4Foamis known to work withbisonversion 2.4 and higher. Version 2.3 compiles but the plugin-functionality does not work correctly. Version 3.0 does not work- flex
- since the introduction of the plugin functions at least
a flex version of
2.5.33is required (2.5.35is the lowest confirmed version)
Both of these are mainstream packages (they are for instance needed
to compile gcc) and should exist on every Linux distribution. Use
the package manager of your distribution to install them and only
if the compilation process of swak4Foam complains about too low
or too high versions compile special version. This can be easily
done by calling
./maintainanceScripts/compileRequirements.sh
in the directory of the sources. This will download a fitting
bison version, compile it and install it in such a way that it is
only used during the compilation of swak4Foam.
swak4Foam tries to keep the requirements on these as low as
possible and sometimes lower versions than the ones reported may
work. If they do please report so.
The version of bison can be checked with
bison -V
The version of flex with
flex -V
wmake all
at the base directory should build all the libraries and tools.
Rerun the command to make sure that there was no problem with the compilation (this should be quite fast and only report libraries being created and some administrative stuff)
Some features (currently only the Python-integration may need
third party software. The paths to these packages can be
configured in a file swakConfiguration (an example file
swakConfiguration.example is provided. There is also a file
swakConfiguration.automatic that tries to automatically
determine the location of Python. It does not work on all systems
and therefor is not enabled by default). If that file is not
present these unconfigured features will not be compiled.
Environment variables that can be set in this file are:
- SWAK_PYTHON_INCLUDE
- Path to the
Python.hfile of the usedpython-installation - SWAK_PYTHON_LINK
- Options to link the
python-library to the library for thepython-integration - SWAK_USER_PLUGINS
- A list of paths separated by
semicolons. These are the directories of libraries with
function-plugins. They are compiled in the course of the
normal
swak-compilation. This makes sure that they are consistent with theswak-release in the case of an update - SWAK_COMPILE_GRAMMAR_OPTION
- Additional compiler switches for
the C-files generated by
bison. Usually used if the default optimization switches are too aggressive and compilation takes to long (then a value like-O0would for instance switch off all optimizations) - SWAK_COMPILE_LEXER_OPTION
- Additional compiler switches for
files generated by
flex. For some compilers (Intel) aggressive optimization when compiling these files may cause uninitialized memory and crashes. This variable can be used to switch off the optimization (usually this fixes the problems) - SWAK_TEST_RACE_CONDITIONS
- Meant to be used only by developers, for performing a verification on whether race conditions occur during parallel compilation, regarding the grammar parsers.
With older versions of 2.0.x (or 2.0 or 2.0.1) it is possible that
the compilation of swakCodedFunctionObject will fail. In that
case remove the last parameter to the
codedFunctionObject-constructor in swakCodedFunctionObject.C
(it is clearly marked by a comment)
Note: This section is very special and won’t be needed by most people
The library libswakPythonIntegration.so links against a specific
version of the python library. In certain circumstances (for
instance the OS of the cluster is different from the one that swak
was compiled on) this python-version is not available on the
target machine. While all other parts of swak will work the
python-integration won’t load on the target machine. To fix this
problem a workaround is provided:
The script maintainanceScripts/makeSpecialPythonLibrary.sh
compiles a special version of the libswakPythonIntegration.so
that is identified by an additional suffix (for instance the
suffix Cluster makes a file
libswakPythonIntegrationCluster.so). That script has to be run
on the target system and needs 3 parameters:
SWAK_PYTHON_INCLUDESWAK_PYTHON_LINK- The suffix
For instance
./maintainanceScripts/makeSpecialPythonLibrary.sh -I/opt/local/Library/Frameworks/Python.framework/Versions/2.5/include/python2.5 "-L/opt/local/lib -lpython2.5" Version2.5
compiles a version for an old python.
To enable the python-integration in libs in controlDict both
python-integrations have to be specified. One of them will fail on
each machine (because the required python-library is not there),
the other one will provide the python-functionObjects.
Note: the special libraries won’t be updated automatically on the target system. Doing so is the responsibility of the user.
If the libraries and utilities are considered stable and the should
be available to everyone (without having to recompile them) the
script copySwakFilesToSite.sh in the directory
maintainanceScripts can be used to copy them to the
global site-specific directories.
The script removeSwakFilesFromSite.sh in the directory
maintainanceScripts removes all these files
from the global directories. The removeSwakFilesFromLocal.sh does
the same for the user directories (this makes sure that no
self-compiled version shadows the global version (which would
lead to strange results)
There is a Makefile attached. make globalinstall compiles swak4Foam
and installs it into the global directories
Note: Due to the order in which library direcories are searched
for with -L a global installation might break the
compilation. If you don’t know what this means: don’t attempt a
global installation
The command build dpkg builds a Debian/Ubuntu package for
the currently enabled OpenFOAM-package. Note:
- it is assumed that the currently used OF-version was also installed by the package manager
- the
devpackage is built but poorly maintained
Changes in the packaging should be done in the branch
debianPackaging of the Mercurial-repository and later be
merged to the default-branch.
Packaging for OpenFOAM 2.x should be done in the branch
debianPackaging_2.x
Note: Due to the problem described with the global installation it might be necessary to deinstall a previously installed package to successfully build a new package
Collection of Libraries
The basis of swak4Foam: the expression parsers with the logic to
access the OpenFOAM data-structures.
None of the other software pieces compile without it.
Also defines a subclass to DataEntry that uses
swak-expressions and a function object initSwakFunctionObject
that might be used if this fails
A collection of function objects that was previously separately available at http://openfoamwiki.net/index.php/Contrib_simpleFunctionObjects.
Provides consistent output of values (on patches and fields) and more.
Implements the infamous groovyBC. A boundary condition that
allows arbitrary expressions in the field-file
Function objects that have no additional requirements. Mainly used for manipulating and creating fields with expressions
- addGlobalVariable
- Adds a variable to a global swak-namespace. Mainly used for debugging and resolving issues where a variable is needed in a BC before it is defined.
- expressionField
- Create a new field from an expression
- clearExpressionField
- Erase a field created with
expressionField - manipulateField
- Modify a field in memory
- createSampledSet
- Create a sampled set that can be used by other swak-entities (mainly boundary conditions)
- createSampledSurface
- Create a sampled surface that can be used by other swak-entities (mainly boundary conditions)
- swakCoded
- Child of the
coded-functionObject that can read and write global variables from and to swak-namespacesAssumes that the
SWAK4FOAM_SRCenvironment variable is set to theLibraries-directory of theswak4Foam-sources - solveLaplacianPDE
- Solve the Poisson equation
\begin{equation}
\frac{∂ ρ T}{∂ t} - ∇ λ ∇ T =
Sexpl + Simpl T
\end{equation}
for
- solveTransportPDE
- Solve the transport equation
\begin{equation}
\frac{∂ ρ T}{∂ t} + ÷(φ,T) - ∇ λ ∇ T =
Sexpl + Simpl T
\end{equation}
for
- addForeignMeshes
- this allows specifying new foreign
meshes. These can be used in subsequent function-objects or
other swak-expressions on
internalFields - foreignMeshesFollowTime
- this allows specifying a list of meshes whose time is set to the current time of the running case
Function objects based on the simpleFunctionObjects-library
(which is a prerequisite for compiling it).
Evaluate expressions and output the results
These classes allow to manipulate the solution. To use these the solver has to be modified.
- expressionSource
- Field that is calculated from an expression. To be used as source-term or coefficient in some solver
- forceEquation
- force an equation to fixed values in selected locations. Has to be used after constructing the equation and before solving
These sources are based on basicSource and can be used
without a modification of the solver (they are only available in
the 2.x version):
- SwakSetValue
- sets values according to a mask or the
mechanism provided by
basicSource - SwakExplicitSource
- Uses the calculated source term on the right hand side of the equation
- SwakImplicitSource
- Uses a calculated scalar-field to add an implicit source term (source is without the actual field)
Starting from OpenFOAM 2.2 this library has additional fvOptions
topoSources for cellSet and faceSet. Can be used with the
cellSet and faceSet-utilities
Implements parsers for the finiteArea-stuff in 1.6-ext. Also
implements groovyBC for areaField and expressionField and
other function objects
Collection of boundary conditions that give standard boundary conditions the possibility to use expression for the coefficients
Contributions to this library are explicitly encouraged. Please
use the Mercurial-branch groovyStandardBCs to groovyify
standard boundary conditions.
Embeds a Python-interpreter.
pythonIntegrationFunctionObject- Executes
Python-code at the usual execution times of functionObjects. The interpreter keeps its state
This library is only compiled if the paths to the Python-Headers
are configured in the swakConfiguration-file (see above)
Function objects that allow the easy addition of lagrangian
clouds to a case. No other libraries from swak4Foam are needed
for this
Additional searchableSurfaces (for use in snappyHexMesh)
which include boolean operations for other surfaces and
coordinate transformations
Driver for functionObjects that implemented entirely in Python
using the pythonFlu-library
Parser for calculating expressions on clouds of lagrangian particles
Library with function objects and plugin functions to work with simple state machines
Library with classes that combine swak with dynamic meshes
Directory with a number of libraries with function-plugins:
- swakFacSchemesFunctionPlugin
- functions with selectable discretization schemes for FAM (only used in 1.6-ext)
- swakFvcSchemesFunctionPlugin
- functions with selectable schemes for FVM
- swakLocalCalculationsFunctionPlugin
- calculations that are local to a cell (Minimum of the face values or so)
- swakMeshQualityFunctionPlugin
- calculate mesh quality criteria like orthogonality, skewness and ascpect ratio
- swakRandomFunctionPlugin
- different random number distributions. Currently only exponential
- swakSurfacesAndSetsFunctionPlugin
- calculates distances from
sampledSurfacesandsampledSetsand projects calculated values from these onto a volume field - swakThermoTurbFunctionPlugin
- Access functions from the thermophysical model and the turbulence model in the current region. Loads the model only if necessary
- swakTransportTurbFunctionPlugin
- Same as above but for incompressible models
- swakLagrangianCloudSourcesFunctionPlugin
- Functions that get informations like source terms from clouds of particles (due to technical reasons this works only for the regular intermediate clouds)
- swakVelocityFunctionPlugin
- Functions that work on the flow field (currently only the local Courant-number)
- swakChemistryModelFunctionPlugin
- Functions that calculate chemistry properties (reaction rates etc)
- swakRadiationModelFunctionPlugin
- Functions that calculate properties of the radiation model
- swakMeshWaveFunctionPlugin
- Functions that use the
MeshWave-algorithm to calculate grid-dependent properties like number of mesh layers
Because of the templating all plugin-functions have to be reinstaniated for new particle classes. The libraries in this directory
- reimplement the functions from
swakLagrangianCloudSourcesFunctionPlugin - the
CloudProxyfor thecloudparser
for special particle classes. These are
- coalCloudAdaptor
- the library
libswakCoalCloudAdaptorthat handels theCoalParcel-class
These libraries have to be included in the libs-entry to
be able to handle these libraries
Utility that allows creation and manipulation of files with expressions
Utility like funkySetFields for areaFields (only works with
1.6-ext)
Sets any field on a boundary to a non-uniform value based on an expression.
Acts without deeper understanding of the underlying boundary condition
Utility to quickly test whether a groovyBC gives the expected results. Writes the specified fields with the applied boundary condition but doesn’t do anything else.
Can be used for other BCs as well
Evaluates expressions that are listed in a dictionary using data that is found on the disc and prints summarized data (min, max, average, sum) to the screen
Calculates the offsets-entry in the polyMesh/boundary-file
according to the specification in a dictionary. Only needed if you
have mapped patches and the regular uniform offset is not enough
for your purposes
Utility that quickly does some quantitative analysis (minimum, maximum, average etc ) on a field on the disc (internal field but also patches, sets, zones, …)
This utility loads specified fields into memory, executes a list of user-specified function objects whose data is then passed to a python script which does the user-specified analysis.
Utility to calculate fields for a lagrangian cloud (or setting it up from scratch)
Utility to write fields with subfields from boundary conditions
like refValue for post-processing
If not otherwise noted cases are prepared by a simple
blockMesh-call.
Note: All the cases here are strictly for demonstration purposes and resemble nothing from the ‘real world’
Note: Due to various changes in the case syntax between OpenFOAM
2.0 and 2.2 (for instance thermophysicalProperties, wall
functions etc) not all of the examples work with all
OpenFOAM-installations “out of the box”. Slight adaptions may be
necessary
Some of the cases use the pyFoamPrepareCase.py-utility of PyFoam
to set up the case for the current OpenFOAM-version
To run on multiple OpenFOAM-versions the cases sometimes have more entries in the dictionaries
Also have a look at Documentation/exampleCompatibilityMatrix.org
to see with which versions which cases should work.
Usually the cases have been derived from regular tutorial
cases. After their first implementation they were only adapted to
run in new OpenFOAM versions but improvements in the tutorials are
usually not ported. The reason is that these are just example
cases for swak4Foam, not best practice examples for OpenFOAM
The old groovyBC-Demos
- Solver
- pisoFoam
- Also demonstrates
manipulateField,expressionFieldandclearFieldfrom theswakFunctionObjects.patchExpressionfromsimpleSwakFunctionObjects.solveLaplacianPDEandsolveTransportPDEfor solving equations,pythonIntegrationwith calculations usingnumpy- Preparation
pyFoamPrepareCase.py
- Solver
- solidDisplacementFoam
- Solver
- interDyMFoam
- Preparation
pyFoamPrepareCase.py
- Solver
- pimpleDyMFoam
- Also demonstrates
swakExpressionwithsurface. Due to a problem described below this currently doesn’t work
- Solver
- pimpleFoam
- Mesh preparation
pyFoamPrepareCase.sh
- Solver
- pimpleFoam
- Mesh preparation
pyFoamPrepareCase.sh- Demonstrates
- Delayed variables to simulate an inflow that depends on the value of the outflow
- Solver
- chtMultiRegionFoam
- Mesh preparation
- Execute the script
prepare.shin that directory - Also demonstrated
patchExpressionandswakExpressionfromsimpleSwakFunctionObjects.
- Solver
- interFoam
- Also demonstrates
- Usage of a
sampledSetdefined in thecontrolDictdo determine the average filling height. Also stored variables for not switching back once the criterion is reached. Global variables defined by a function object
- Solver
- interFoam
- Description
- Winner of the
swak4Foam-competition at the 6th OpenFOAM-Workshop (2011). By Peter Keller
- Solver
- potentialFoam
- Description
- Demonstrates the use of
groovyBwithpotentialFoam(also a problem connected with that). Provided by Martin Backer
- Solver
- interFoam
- Preparation
- run
pyFoamPrepareCase.py - Description
- Demonstrates the use of 2-dimensional lookup tables. For the initialization as well as the boundary condition
Example dictionaries for funkyDoCalc
Example dictionary for funkySetFields
Example dictionary for funkySetBoundaryFields. Sets nonsense
boundary conditions for the world famous damBreak-case
Demonstrates usage of expressionSource
Due to differences in the original interFoam-solver this doesn’t
work on certain OpenFOAM-versions (most specifically
1.6-ext). The current solver works with 2.1. For older
OF-versions use the sources labeled _pre2.1.
The only modifications to the original solver are found at the end
of createFields.H and in UEqn.H (the added source terms).
Demonstrates usage of forceEquation
Due to differences in the original interFoam-solver this doesn’t
work on certain OpenFOAM-versions (most specifically
1.6-ext). The current solver works with 2.1. For older
OF-versions use the sources labeled _pre2.1.
The only modifications to the original solver are found at the end
of createFields.H and in UEqn.H (the fixing of the velocities).
Slightly modified version of interFoam. Adds a source term to
the momentum equation. The source term is an expression that is
defined at run-time
Demonstration case for it.
- Preparation
- Run the script
prepare.shto prepare the case
Demonstration of the finiteArea-stuff that works with 1.6-ext
Variation of surfactantFoam that adds an expressionSource
Demonstration case
- Preparation
- Use
pyFoamPrepareCase.py - Solver
surfactantFoam(without source term) orswakSurfactantFoam- Demonstrates
- FAM-specific
swakExpressionsandgroovyBC(as well as theexpressionSource)
Cases that demonstrate swakSourceFields
- Solver
- rhoPimpleFoam
- Mesh preparation
- Execute
pyFoamPrepareCase.py . - Demonstrates
- Simple expression sources (adds a heat source to the solid)
- Solver
- chtMultiRegionFoam
- Mesh preparation
- Execute
pyFoamPrepareCase.py . - Demonstrates
- Getting the residuals of the matrix with the
matrixChangeBeforeandmatrixChangeAfterfvOptions
Cases that don’t have a groovyBC
- Solver
- rhoPorousMRFSimpleFoam
- Mesh preparation
- Execute the
makeMesh.sh-script in that directory. If you want to run in parallel call thedecomposeMesh.sh-script with the number of processors as an argument - Demonstrates
- Usage of the
swakTopoSources. Compares different approaches to evaluating with theswakExpression-functionObject. Also an example dictionary that demonstrates the use offunkyDoCalc. Demonstrates “live” comparing to another case using foreign meshes
- Solver
- rhoPorousMRFPimpleFoam
- Mesh preparation
- Execute the
makeMesh.sh-script in that directory. If you want to run in parallel call thedecomposeMesh.sh-script with the number of processors as an argument - Demonstrates
- The same as
angledDuctImplicitbut also the output of temporal changes
- Solver
- interFoam
- Case preparation
- run the
pyFoam-utilitypyFoamPrepareCase.py - Demonstrates
- Usage of a sampled surface to track the interface in a VOF-simulation
- Solver
- interFoam
- Case preparation
- run the supplied script
prepareCase.sh - Demonstrates
- Emulate a “moving gravitation” by using the
manipulateField-functionObject to recalculateghandghf
Demonstrates initializing a case with initial conditions that approximate the real flow.
- Solver
- reactingFoam
- Case preparation
- run
pyFoamPrepareCase.py. Caution: this has to be done every time before running the case because the initialized fields are rewritten - Demonstrates
- Demonstrates setting calculated initial conditions with functionObjects
Demonstrates the use of funkyWarpMesh and post-processing on
bended pip geometries
- Solver
- simpleFoam
- Case preparation
- Run
prepare.sh
Case to demonstrate various things about cell and faceSet
- Solver
- interFoam
- Case preparation
- Run
pyFoamPrepareCase.py .
Cases that were shown in some presentations
- Solver
- interFoam
- Case preparation
- run the
prepareCase.sh-script - Description
- The case described on the slides of the
talk about
swak4Foamat the OSCFD-conference 2012 in London - Demonstrates
- Boundary conditions, function objects, global variables and delayed variables
A 2D-variant of the above case
- Solver
- twoPhaseEulerFoam
- Case preparation
- run the
prepareCase.sh-script - Description
- Simulate a sand-monster from the StarWars-movie “Return of the Jedi”
- Demonstrates
- Use of
funkySetFields,groovyBCand functionObjects for lagrangian particles
- solver
- simpleFoam
- Case preparation
- run the
prepareCase.sh-script - Description
- Simulates two landSpeeders (as seen in the StarWars-movie “A New Hope”)
- Demonstrates
- Advanced searchableSurfaces (for
snappyHexMesh), functionObject for passive scalar, functionObject to calculate distributions
Demonstrate the integration of Python. Mostly using PyFoam but
also with pythonFlu
- Solver
- simpleFoam
- Demonstrates
- Usage of
PyFoamto manipulate thefvSolution-file during the run (possible application: unphysical initial conditions cause the run to fail during startup with “normal” relaxation values)
- Solver
- simpleFoam
- Demonstrates
- Usage of the
pythonFlu-integration to find the point where the recirculation behind the step ends. Also tries to plot the result using thematplotlib-library
- Solver
- twoPhaseEulerFoam
- Demonstrates
- Usage of
PyFoamto read the direction of gravity and feeding it into agoovyBCvia global variables - Case preparation
- Just call
funkySetFields -time 0
- Solver
- chtMultiRegionFoam
- Demonstrates
- Building the specification of function objects at run-time via a Python-script
- Solver
- simpleFoam
- Demonstrates
- Using a python-script to dynamically generate multiple function objects (sampled surfaces). Using stack-variables to calculate the results and write them. Using a stored stack-variable to monitor the pressure at a point and stop the run if the pressure didn’t change there for the last 50 iterations
Demonstrates working together with the coded-stuff in OpenFOAM 2.0
Examples for the functionObjects that can solve Partial
Differential equations
- Solver
- laplacianFoam
- Demonstrates
- The usage of the
functionObjectthat solves the laplacian (Poisson) equation and (hopefully) that it gets the same result as the native solver - Case preparation
pyFoamPrepareCase.py
- Solver
- scalarTransportFoam
- Demonstrates
- Solving additional transport equations
These examples test the source terms based on basicSource. They
only work with OpenFOAM 2.x and all use the simpleFoam-solver
- Demonstrates
- Fixing the values of the velocity in a region
with
SwakSetValues
- Demonstrates
- Implementing a simple porous plug by adding the
Darcy-term as a source term with
SwakExplicitSource
- Demonstrates
- Same as
pitzDailyWithExplicitPoroPlugbut with an implicit source term withSwakImplicitSource
Stuff that has to do with lagrangian particles
Tests for the functionObjects that create and evolve a cloud of
particles (library simpleLagrangianFunctionObjects)
- Solver
replayTransientBC- Mesh preparation
pyFoamPrepareCase.py .- Demonstrates
- 3 clouds (kinematic, reacting, solidParticle). Loading of a thermophysical model with a functionObject. Plugin functions for information about the clouds
- Solver
- rhoPimpleFoam
- Demonstrates
- Thermo-cloud. Functions for lagrangian particles
- Solver
- icoFoam
- Demonstrates
- Simplest way to add particles to a case
Testing the cloud-parser for lagrangiant particles
- Solver
- reactingParcelFoam
- Demonstrates
- Adding evaluations on the cloud to a regular case
Variation of the tutorial case
- Solver
- coalChemistryFoam
- Demonstrates
- creating new clouds with
funkySetLagrangianFieldand evaluations on clouds during the simulation - Mesh preparation
- run the
pyFoamPrepareCase.py .script to set up the mesh and the fields
Examples for the use of the simpleSearchableSurfaces-library.
- Solver
- simpleFoam (alternatively use the
caseRun.sh-script) - Case preparation
- Script
caseSetup.shis provided - Demonstrates
- Using the same STL-file more than once in a case by applying coordinate transformations. Note: the physics of this case are more than questionable as the frame of reference for both motorbikes is wrong
- Solver
- interFoam
- Case preparation
- Use
pyFoamPrepareCase.py - Demonstrates
- Boolean operations on STL-files
- Solver
- electrostaticFoam
- Case preparation
- Script
caseSetup.shis provided - Demonstrates
- Boolean operations with regular surfaces
Physics of the case not as expected (charge-distribution)
Demonstrates the use of function objects that change the numerics during the run
The regular simpleFoam-tutorial. Modified so that it switches
to higher relaxation factors during the run
simpleFoam-tutorial. Uses state machines to change the
discretization periodically
Demonstrate the usage of state machines
The case is only an excuse for the state machines
- Running
replayTransientBC -allowFunctionObjects- Case setup
pyFoamPrepareCase.py
Examples that demonstrate dynamic mesh applications
Variation of a tutorial case where the oscillation has been replaced by an expression
- Solver
pimpleDyMFoam- Case setup
pyFoamPrepareCase.py- Demonstrates
- The
swakMotionfunction forsolidBodyMotion
- Solver
interDyMFoam- Case setup
pyFoamPrepareCase.py- Demonstrates
- The
swakMotionfunction forsolidBodyMotion
- Solver
pimpleDyMFoam- Case setup
pyFoamPrepareCase.py- Demonstrates
- The
groovyCyclicACMIpatch type
- Solver
compressibleInterDyMFoam- Case setup
pyFoamPrepareCase- Demonstrates
- The
groovyCyclicACMIpatch type. State machines.funkyWarpMeshutility
Simple test cases for specific features. The names of the
directories should give you a hint what is tested there. Most of
them don’t need a real solver but replayTransientBC or
scalarTransportFoam.
Note: for some features these cases are the only example there is. Sorry
Testing of different seeds for the rand-function. Also tests
the randFixed-function
Simple geometry for testing function objects with AMI. “Execute”
with replayTransientBC, pimpleFoam or pimpleDyMFoam
Features can be “switched off” with pyFoamPrepareCase.py. What
can be switched on is a location dependent pressure jump on one
of the interfaces implemented with groovyBCJumpAMI
These are cases provided by users to demonstrate bugs. Not maintained nor documented and may be removed at any time
Undocumented scripts used for maintaining swak4Foam. If you
don’t understand them, don’t use them
Additional documentation. Most written in org-mode
Current contents:
- swak4FoamReference
- Reference manual of swak4Foam. Especially concepts like expression syntax and parameters
Scripts and configuration to test for a release in a virtual
machine using vagrant. Also to be used for packaging
Patches that have to be applied to releases to get swak4Foam to work with them. These are only needed to fix problems of the distributions
The preferred place for bug reports is http://sourceforge.net/apps/mantisbt/openfoam-extend/search.php?project_id=10&sticky_issues=on&sortby=last_updated&dir=DESC&hide_status_id=90
A sourceforge-account is required for reporting
Please always report the FOAM-version you use. As OpenFOAM-dev
is a moving target only bug-reports that add fixes are handled for this.
If you’re reporting a bug about the compilation please run
Allwmake twice and only report the messages from the second
run. This makes analyzing the log easier as only the unsuccessful
commands will be reported.
If the problem seems to be a missing library rerun the compilation to make sure that there wasn’t a problem with that.
Contributions to to swak4Foam are most welcome. If you want to
contribute clone the Mercurial archive of the sources
hg clone http://openfoam-extend.hg.sourceforge.net:8000/hgroot/openfoam-extend/swak4Foam
Change to the branch that you want to improve (usually default)
and create a new branch
hg branch <branchName>
where <branchname> is an easily identifiable name that makes the
purpose of the branch clear (for instance
hotfix/WrongRandomFunction or feature/HyperbolicFunctions). Don’t
work on the default branch or any other branches that are not
“yours”. Such contributions will not be merged
Once development on the branch is finished export the relevant changesets with
hg export <nodeID>
(nodeID being the ids of “your” changesets) and send them to the
maintainer (or attach them to a bug report on Manits). The changes
will be reviewed and merged into the default branch (do not
attempt to do this yourself). Patches generated with hg export
make sure that all changes are attributed to the original developer
(you).
An alternative would be the bundle command. Just do
hg bundle <bundlefile>
and then send the bundlefile. This will include all commits
that are not in the upstream repository and will allow similar
inclusion in the upstream as export.
Once you have proven by successfully submitting changesets via hg
export you can ask for write access to the mercurial repository.
Only if you got through Mercurial it can be ensured that your contribution is recognized (if you want to stay anonymous send patches).
These topics may be “new” for the average OF-developer:
- Mercurial
- A short tutorial on this can be found at
http://mercurial.selenic.com/guide/. If you already
know
gitthe http://mercurial.selenic.com/wiki/GitConcepts may be enough for you - bison/flex
- This pair of compiler generator tools generate the
parsers for the expressions. Google for a tutorial
that looks promising to you.
For a short example that shows how a new function was added to two parsers have a look at this changeset that added the
cpu()-function to the field and the the patch-parser (usually you’ll have to write a new method for the driver too):
hg diff -c 8604e865cce6
Currently the main branches are:
- default
- The main branch. This is the brancht that the general public will receive. It compiles under OpenFOAM 2.0 and higher
- debianPackaging
- Branch for generating new Debian-packages of
swak4Foam. If somebody wants to “inherit” this: contact the maintainer - develop
- Actual development branch
As an experimental feature distributed bug-tracking was introduced using the Artemis-extension for Mercurial (see http://hg.mrzv.org/Artemis/). An up-to-date version can be installed by
hg clone http://hg.mrzv.org/Artemis/
somewhere and installing the plugin by editing .hgrc.
This is not the official bug-tracker for swak4Foam. It is used
for keeping track of new features that are to be introduced to
swak4Foam and may be discontinued if the experiment proves to be
unsuccessful.
The repository comes with a .hgflow-file that is set for the
hgflow-extension found at
https://bitbucket.org/yujiewu/hgflow/wiki/Home (there are multiple
branches of this extension. This seems to be the most up-to date
and still under active development)
In the future this repository will try to stick to the model described in http://nvie.com/posts/a-successful-git-branching-model/
swak4Foam is free software; you can redistribute it and/or modify it
under the terms of the GNU General Public License as published by the
Free Software Foundation; either version 2 of the License, or (at your
option) any later version. See the file COPYING in this directory,
for a description of the GNU General Public License terms under which
you can copy the files.
The following list is not complete. If the Artemis extension (see above) is installed then
hg ilist
gives a more up-to-date list
It seems that with moving meshes sampledSurfaces don’t get
updated. This seems to be a problem with OpenFOAM itself (the
regular surfaces-functionObject doesn’t get updated. This is
currently investigated
Apart from patches and internal fields the support for interpolation from cells to faces (and vice versa) is incomplete as well as point fields (although they are supported in the grammar)
This is especially evident for the funkyDoCalc-example
Not really bugs, but stuff that bugs me
This is necessary because of bison. Investigate possibilities to
replace these by tmp and autoPtr
valgrind reports some lost memory for stuff that is not directly
allocated by swak4Foam (in OpenFOAM-sources)
Will investigate. Relevant places are marked by comments in the
code. Also the construction of sampledSet seems to loose memory
Currenly problematice parts seem to be:
- update and
magSf-calculation ofSampledSurface(marked inSampledSurfaceExpressionDriver.C) - Python interpreter (but no calls in swak were found in the stack-trace that could be responsible)
Before OpenFOAM 2.1 the inner product of two symmetric tensors was a symmetric tensor. Since 2.1 it is a general tensor. As the general treatment in the grammar would be confusing currently the this product was removed from the grammar and therefor will not be correctly parsed
The same problem that was mentioned in https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=130 is also true for subsets. But as the interpolation is not implemented for most subsets this will be postponed
The tab-completion does not work except for up-to-date versions of
IPython. This seems to be a problem with the readline-library
inside an embedded Python. Low priority
If the commsType is set to blocking then the MPI-communications
of groovyBC cause problems in MPI and a fatal error.
Currently the only workaround is to edit
$WM_PROJECT_DIR/etc/controlDict so that a different commsType
is used (nonBlocking or scheduled)
Older Foam-versions had the problem that when the surface changes
the size then certain values (especially the mag are not properly
recalculated).
This causes this bug: https://sourceforge.net/p/openfoam-extend/ticketsswak4foam/231/
The bug can not be fixed in swak4Foam but has to be fixed in the
Foam-Distro
Currently only the data from scalar fields can be correctly
parsed. If vector-fields are specified the function object fails
First Release
New release Most important changes
Now expressions for the field on a sampled surface can be
evaluated. All sampledSurfaces offered by OpenFOAM now can be
used
The variables entry (most notably used in groovyBC and
swakExpression) now can be a list of strings. This allows some
kind of “formatting” (one expression per line) and should improve
readability
These can copy the libraries and utilities to the global
installation (for those who think that the swak4Foam-stuff is
stable enough and want to ‘bless’ all users at their site with
it). Note that any local installation still takes precedence
(because $FOAM_USER_APPBIN is before $FOAM_APPBIN in the
$PATH
This allows the inclusion of other parsers with the regular
swak4Foam parsers and include them seamlessly with the
variables-mechanism for ‘externals’ (in other words: you can add
your own parser in a separate library without having to change
anything about the overall swak4Foam, but it behaves as if it
was part of it)
Now there is support for the finiteArea-library found in
1.6-dev. The support is found in a separate library
swakFiniteArea. It has
- a parser
faFieldforareaFields - a parser
faPatchfor patches ofareaFields - a variant of
groovyBCfor these patches - a computed source
faExpressionSource - Function-object-variants for
areaFields:clearExpression,expressionFieldandmanipulateField. These work the same as theirvolField-counterparts
See https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=49
See https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=44
New features and changes are (this list is not complete):
Like funkySetFields for finiteArea. Also writes out a volume
field for easier post-processing
Makes it easier to use the groovyBC-machinery for other boundary
conditions. Two standard boundary conditions were
groovified. Others may follow
If no simpleFunctionObjects are present they can be downloaded
by a script.
Also scripts to handle global installations of swak4Foam
A class to force equations to certain values according to expressions
Utility does calculations on saved results and outputs single numbers (min, max, sum, average) to the terminal. Can be used for reporting or validity checks
Crude packaging for Debian
A single-argument function can be specified as a piecewise linear function. Basically works like timelines but the argument can be something else (not only the time)
Variables that store their values between time-steps. Applications are statistics or switches
Sampled sets can now also be used as en entity on which calculation is possible.
This is the first release that officially supports OpenFOAM 2.0
Also it is the first release that incorporates the
simpleFunctionObjects-library
- These two functions now can receive an integer seed that determines the pseudo-randooom sequence generated by these functions
- Two functions
randFixedandrandNormalFixedwere added. While the usualrandfunctions generate a different result at every time-steps for these functions the pseudo-random sequence is determined only by the seed (not by the timestep)
Take the bigger/smaller of two fields. Helps avoid ?:-operations
Application: If the results of the calculation are only needed in ParaView
- Use
autoPtrfor sets - Update sets that change in memory or on disc
Fixed by Petr Vita
Calculated boundaries were
- Packaging information for the currently used OF-version is
generated (allows a separate
swak-package for every OF-version - Submission to launchpad added
Now install to FOAM_SITE_APPBIN/LIBBIN
Uses the usual -region-option. Looks for a separate dictionary
in the system-directory of that region
This can be switched on using the allowFunctionObjects-option
Allows the execution of Python-Code in a functionObject
This feature is still experimental and the organization of the libraries is subject to change
It is now possible to define variables that are ‘global’: They can be read in any entity.
Currently these variables can only be uniform.
To access global variables the specification-dictionary has to
have a wordList named globalScopes. The scopes are searched
in that order for the names of global variables. Having scopes
allows some kind of separation of the variables
Adds a functionObject swakCoded that extends the
coded-functionObject to read and write global variables
Added a boundary condition than allows to only fix the
values. This should help to avoid problems with cases that don’t
like mixed (on which the regular groovyBC is based)
Two function objects that solve Partial Differential Equations during a run have been added:
- one that solves a laplacian (Poisson) equation
- one that solves the transport equation for a scalar
The relevant coefficients (including explicit and implicit source terms) can be specified using expressions
Added a script that takes the current sources, copies them into
the appropriate places of a OpenFOAM-installation and slightly
rewrites them to compile in this place. What happens then
(committing them into the repository or just plain compilation)
is up to the maintainer
As many parts of swak4Foam depend on it the
simpleFunctionObjects have now been absorbed into
swak4Foam. They can still be compiled on their own
If a variable is defined and the patch which it is defined on doesn’t have any faces the variable is reported on that processor as not existing and the whole run fails
Fixed according to a suggestion by Andreas Otto. Now runs again (used to crash some time-steps into the beginning)
The Allwmake-script now checks for the correct bison-version
(and the existence of bison) and fails if it doesn’t seem to be
the right one
To allow distinguishing different OF-versions as discussed in the
bug report
http://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=114
the Allwmake-script now generates a header file
foamVersion4swak.H that defines the symbols
FOAM_VERSION4SWAK_MAJOR, FOAM_VERSION4SWAK_MINOR and
FOAM_VERSION4SWAK_PATCH
- now can also produce surfaceFields
- full support of
tensor,symmTensorandsphericalTensor
- now can also produce edgeFields
No support for tensors yet
If necessary (for instance swakExpression-functionObject) the
storedVariables are written to disc (into a subdirectory
swak4Foam of the timestep) and are reread at the start. This
allows consistent restarts (for instance if a flow was summed
using the variable) if the expressions stay the same.
Data files can now be written without brackets but each component on its own. The number of entries in the header is not adjusted
For drivers that don’t have access to a fvMesh a default mesh
exists. This default mesh is defined by the first fvMesh that
is used during the construction of any driver.
Definition of the default mesh can be forced using the
initSwakFunctionObject (see the test case flowRateAngledDuct)
Due to the refactoring of the FieldDriver now phi can be
specified by a general expression (instead of ‘only’ a
field-name)
Can write surfaceVector and surfaceScalar-Fields. Condition
has to be consistent
expressionField and manipulateField now can create or modify
surfaceFields
funkySetFields and the function objects expressionField and
manipulateField now also work with the three tensor-types
If the expression evaluates to a surfaceField then this is used
as a flag whether or not the face is in the faceSet. If the
expression evaluates to a volScalarField then the old semantic
applies (faces are in the set if one cell is true and the other
is false).
This only works for internal faces
If there is an entry globalVariables then this dictionary is
used to set the variables
Calculates variables and then pushes them to a global namespace
New option added that generates a phi field with value inletOutlet happy
The functionObject dumpSwakExpression dumps the complete
results of a swakExpression to file at each timestep. This
produces huge files and is therefor not endorsed
Add the options allowFunctionObjects and addDummyPhi to
execute functionObjects and add a phi-field (for fields that
require these)
Based on the directionMixed boundary condition this allows to
set a boundary condition as a Dirichlet-condition only in certain
directions while in the other directions it is a
gradient-condition
Boundary condition that imposes a jump in the value on a cyclic
boundary condition pair (based on jumpCyclic). Only works for
scalar values
Setting the option outputFileMode to csv writes
CSV-files. The option-value foam is the default (old style). The
option-value raw writes the values delimited by spaces (no
brackets for vectors and tensors)
If a submesh is not yet in memory and the option searchOnDisc
is set, the mesh is automatically read into memory and kept there
The simpleFunctionObjects-library now has a number of
functionObjects that allow the conditional execution of a list of
function objects.
These are
- executeIfExecutableFits
- if the name of the executable fits a regular expression the function objects are executed
- executeIfObjectExists
- if a named object exists (or alternatively: doesn’t exist) in the registry execute the function objects. Type checking also implemented
- executeIfEnvironmentVariable
- execute if an environment variable satisfies a certain condition (exists, doesn’t exist, fits a regular expression)
- executeIfFunctionObjectPresent
- execute if a specific functionObject is present. This can help prevent failures if a functionObject is missing for technical reasons
In addition the simpleSwakFunctionObjects-library has
- executeIfSwakObject
- Evaluates a logical swak-expression. The results are either accumulated using logical or (if one value is true the result will be true) or logical and (all values have to be true)
The pythonIntegration-library has
- executeIfPython
- Evaluates a Python-code-snipplet that returns a value. If this value is “true” in Pythons standards then the functionObjects are executed
simpleFunctionObjects has an additional function object that
reads the direction of gravitation. The purpose is to assist
boundary conditions like buoyantPressure that rely on it to
work. Best used together with conditional function objects (“If
g is missing ....”)
Solve transport and laplacian equation
This is defined in the swak4FoamParsers-library. The class
needs a default mesh defined to construct the driver. Definition
of the default mesh (if no other driver was constructed in some
function-object or by a groovyBC) can be forced using the
initSwakFunctionObject (see the test case flowRateAngledDuct)
Similar to the surfaceFields in funkySetFields
The Utilities failed with the Intel-compiler. Compilation now
falls back to good old g++
Because the tokens were not defined in the flex-files getting
tensor components with tensor.xx did not work. Fixed
Because surfaceFields know no zeroGradient the template
makeConstant did not work
Change so that the field gets temporarily loaded to calculate the
gradient on the patch. Same for internalField and
neighbourField
The reason is that groovyBC usually doesn’t get evaluated
during construction. The reason is that it is hard to tell
whether all required fields are already in memory. The current
fix is a workaround: setting evaluateDuringConstruction to
true forces the BC to be evaluated during construction
Extra evaluation of boundary condition that should fix the
problem with calculated patches causes funkySetFields to fail
with stock boundary conditions if not all fields are present in
memory
This boundary condition will be removed in future releases
because the base class now supports the more general
DataEntry-class for which a swak-subclass exists
To distinguish the output of various instances of
functionObjects from the simpleFunctionObjects-library in
multi-region cases the screen-output is prefixed with the region
name. For the default region nothing changes. Directory names
stay the same as they are unambiguous anyway (they contain the
name of the functionObject)
For fields (not expressions!) the value at a previous timestep
can be gotten via oldTime(field) if that information exists
(also for funkySetFields if the corresponding file field_0
exists.
For fields that support it (basically volume-fields) there is
also a ddt-operator that calculates the explicit
time-derivative (if information about the last timestep exists)
Currently implemented for
- internalFields
oldTimeandddt- patch
- only
oldTime - cellSet,cellZone
- only
oldTime - sampledSurface,sampledSet
- only
oldTime - faceSet,faceZone
oldTime- internalFaFields
oldTimeandddt- faPatch
- only
oldTime
If there is no old time value stored and in the parser dictionary
the parameter prevIterIsOldTime is set, then the previous
iteration value is used as the old time.
Based on the directionMixed boundary condition this allows to
set a boundary condition as a Dirichlet-condition only in certain
directions while in the other directions it is a
gradient-condition
Note: this should have been in the last release but was forgotten to merge into the default branch
Boundary condition that imposes a jump in the value on a cyclic
boundary condition pair (based on jumpCyclic). Only works for
scalar values
Note: this should have been in the last release but was forgotten to merge into the default branch
The functions minPosition and maxPosition return the position
of the minimum or the maximum of a scalar field
This is implemented for all field types
Now can read and generate pointFields.
Detailed features (apart from the standard symbols) are:
- Function
pointgenerates a constantpointScalarField - Function
pts()returns apointVectorFieldwith the point positions - Functions
pzoneandpsetgenerate logical fields according to existing pointZones or pointSets - Functions
interpolateToCellandinterpolateToPointinterpolate from pointFields to volFields and from volFields to pointFields
Utilities and functionObjects affected by this are
funkySetFields- new topoSource
expressionToPoint expressionFieldandmanipulateFieldnow can deal with pointFields
The faField-parser now supports tensors, symmetric tensors and
spherical tensors.
Not all operators are supported because the are not instantiated in 1.6-ext
These variables are added in the namespace to ease the writing of Python-code whose output is consistent with OF
- timeName
- Name of the current time as a string. Allows the construction of directory names
- outputTime
- Boolean that indicates whether this is a timestep where OpenFOAM will write output
The missing operators from the fvc-namespace have been added to
the Field-parser. These are
d2dt2- for all volumeFields
flux- for all volumFields. Needs a surfaceField as a first argument
meshPhi- for volume-vector-fields. Optional with a scalar-field that acts as the density as the first argument. Only works in the context of a solver with a dynamic mesh and hasn’t been tested yet
The only missing operators from the fvc-namespace are
volumeIntegrate=/=domainIntegrate. These have been omitted as
they are trivial to implement using other functions
Thanks to patches supplied by Bruno Santos (see http://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=105) compilation of the libraries is now possible in parallel
Releases up to now got a version number. Utilities now report the version number. This should make it easier to find out whether problems are due to an old version
Still looking for a way to do that for the libraries (so that they will report it if dynamically loaded)
make dpkg now genrates also a valid package if the current
OpenFOAM-installation is not installed using the dpkg.
For parallel runs the content of the caseDir-variable changed
and a few variables have been added
- caseDir
- in parallel runs now points to the
FOAM_CASEinstead of the processor subdirectory - systemDir
- points to the global
system-directory - constantDir
- points to the global
constant-directory - procDir
- in parallel runs points to the processor-subdirectory of the current CPU
- meshDir
- The mesh data (of the current processor in parallel runs)
- timeDir
- Directory where data would be written to at the current time (processor dependent)
In parallel runs the user must set the isParallelized to true
if the parallelMasterOnly is set to false.
With that he indicates that in his opinion the Python-code has no bad side-effects in parallel runs and that he doesn’t blame swak4Foam if anyting bad happens
As reported in
https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=119
due to a change the way the PISO-loop is treated the
interFoamWithSources and interFoamWithFixed don’t compile
with 2.1 anymore.
To avoid #ifdef in the solver sources there is now a separate
set of sources (labeled pre2.1) for older versions. The regular
sources work with 2.1 (and hopefully the following)
Function-objects only work with the
while(runTime.loop())-construct in 2.1. The utility now uses
this.
Bug reported: http://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=124
An expression like 2*U did not work for the field U. Reason
was that the registry already held an object called U (the
dictionary representation of the field) and therefor refused to
load/register another U.
Has been fixed by de-registering the dictionary U immediately
after loading.
The gradient for a vector field (result: a tensor field) was not calculated. It is now part of the grammar
tr, inv and det were not working for some tensort types in
1.6-ext. The parser now fails if such a combination is
used. Works OK for other OF-versions
Also introduced a workaround for certain operators not being properly defined for pointFields (by using the internal fields)
These symbols could not be used as field names because they were used for the components of vectors and tensors
Now these names are only used if the .-operator asks for a
component. This is implemented for these parsers
- FieldValues
- PatchValues
- SubsetValues (all Zones, sets and samples)
- finiteArea-Parsers: faPatch and faField
All parsers except the field-parser were missing the access to tensor components in the grammar
As mentioned in
https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=130
it was not possible to construct a point-vector field using
vector(toPoint(1),toPoint(1),toPoint(1)). Same for tensors
The error message in funkySetFields that was issued when a
field is supposed to be created was not very helpful (something
about the field currently being an IOobject)
This function was reported missing on the message board
The composed objects got their size from the current parser, not the components. This resulted in a segmentation-fault for pointFields
Preprocessor symbol linux unknown. Replaced with __linux__
Now handles bad or non-existent filenames for dictionaries to track
Fix provided by Martin Beaudoin
This version is needed for the reentrant parsers. 2.5.33 may
work but is untested. Version 2.5.4 which is on some old
systems definitely does not work
Version 2.3 compiles but there is an offset-problem with the locations that breaks the Plugin-functionality
Mac-users will have to install bison from another source (for
instance MacPorts)
On Ubuntu /bin/sh is something else and the scripts fail.
Hardcode to /bin/bash
This script (which was removed long ago) was still referenced in
the Makefile.
grad and other operators from fvc added dimensions to values
that were supposed to be dimensionless. This has been fixed
Due to a typo the constructed condition field was too short for surface-fields (too long for volume-fields, but that didn’t matter)
The field-driver created patch fields there as calcuated when
zeroGradient would have been more appropriate
A SortableList was used which meant that the vector with the
flip values was not in the correct order
This problem was due to a non-special treatment of faces on the
boundary. Fixed (for faceZone as well).
Also boundary faces are now honored in expressionToFace if the
expression is a surface-field (for the volume-field logic
boundary faces will never work)
The reason was that during construction refGradient, refValue
etc were not read correctly (if present).
This is now fixed in groovyBC and the other BCs (groovyBC for
pointFields and groovyBCDirection)
The Lexer correctly identified the variable but the getField
method did not know how to get it.
Fixed
If no condition was evaluated the utility generated a pseudo-field of the wrong length
For some operations in the Field-driver the
calculated-patches had the value
The FaField-driver did no fixing of the calculated-patches at
all.
This is fixed
Reported in http://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=150
Added the sqr at the right place to the grammars. Also some
other missing tensor operations (dev and symm).
Patch fields were not copied any no correctBoundaryField was
called for technical reasons.
Fix: values copied by hand
Introduced a preprocessor symbol that allows using sortedToc on newer versions
This was due to a strange () (still don’t know what happened there)
The strings of parsed IDs were not properly deleted. Funnily this was done correctly in the Patch and the Subset-driver. Also for timelines-
Also fixed a leak with the labels of plugin-functions that was present with all drivers
Reported by Oliver Krueger that on systems where /bin/sh is not
a bash anymore (newer Ubuntu and SuSE) the sourcing of
theFiles.sh doesn’t work anymore.
Fixed and moved all the files to the maintainanceScripts-folder
Added. Diag had to be reprogrammed as it is not implemented for fields (probably for performance reasons).
Also some tensor operators were missing (probably lost during copy/paste)
Reported in https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=153
Fixed by removing all file pointers if the number of patches changes
Spaces in the list of variables made the reading fail because words can’t contain spaces. For instance
"var =T*2;"
Now all the spaces are removed before assigning to variables. This will also remove spaces on the “inside” thus making
"v ar =T*2;"
the same as the above expression. But it is unlikely that the call will be used in this way
These valid div-operations were missing from the grammar:
- Divergence of a volume-tensor (all three kinds) producing a vector
- Divergence of a surface-tensor (all three kinds) producing a volume-tensor
Fields created by that function object were written with the value from the timestep before because the regular write occurs before the execution of the function objects.
Fixed
Now an initial value is required (instead of the default empty string which caused parser failure)
Reason is that during the calculation of the variables dimensions are checked.
Now the functionObject switches the checking off. But a more general solution is desirable
The functionObject does not write (and calculate) the field at the last timestep.
Fixed with an one-liner
Reason was an uninitialized valueFraction which sometimes has
values that cause a floating point exception. Fixed
Because size() was equal to the expected size on some
processors. Not on all. Now the branch is taken if the size is
equal on all processors
Fields were not written after the boundary condition was updated. Now they are
The topology operators expressionToCell, expressionToFace and
expressionToPoint now support variables and the other
supporting keywords if being constructed with a dictionary (for
instance from the topoSet-utility)
Usually the manipulated version of the fields is not written as
the manipulation happens after writing. The option
writeManipulated enforces writing.
Writing is not the default behavior to avoid side-effects
The function onPatch(name) returns a surface-field that is name.
The function internalFace() is
Now the second argument to the pow-function can be a
non-constant
The expression A.T() transposes the tensor A (for symmetrical
and spherical tensors it leaves them untouched)
If no field I is defined then this is used as the unit-tensor
The unary operator * calculates for tensors and symmetrical
tensors the hodge dual
The optional entry useFunctionObjects switches on the execution
of function objects during the calculation
The optional entry addDummyPhi creates a phi-field
The dimensions-entry is now read at the same time the variables
are read (this should work for all programs/functionObjects where
the parser is not constructed using a dictionary but the
dictionary is later searched for the variables-entry)
This allows easy extension of the functionality of swak4Foam
without modifying the grammar files.
The way it works is that new functions are added to a runtime-selection table. If the grammar can not resolve a symbol as a built-in function or a field (but only then) it looks up the name in this table and evaluates the function. Parameters are parsed separately and can be:
- primitive data types
- integer, float, string and word
- swak-expression
- an expression parsed by one of the swak-parsers. The type of this expression does not necessarily have to be the same as the one of the ‘main’ expression.
The first time a plugin function is searched swak4Foam prints a
list of all the available functions of this type. Information
included is the return type and the types of the parameters
(these include the parser used, the expected type and a parameter
name).
Libraries with plugin-functions are added via the libs-entry in
the system/controlDict
A number of plugin-libraries are already included covering these topics:
- Evaluation of functions of the turbulence, transport or thermo model
- Different random number distributions
- Functions to “project”
sampledSetsandsampledSurfacesonto a volume-field - Execute explicit discretization functions (like
grad) but select the used scheme in the function instead of using the value fromfvSchemes - Calculations of the mesh quality (same way
checkMeshdoes) and return as fields - Do calculations locally on a cell (like the maximum on its faces)
- Get the source fields and other properties from lagrangian clouds based on the basic intermediate cloud classes (Kinematic, Thermo, Reacting, ReactingMultiphase)
It has been tried to make the names unique instead of short. Usually function names from one library are prefixed with the same short string.
The new dynamicFunctionObjectListProxy in the
simpleFunctionObjects can generate a functionObjectList from
a string and execute them during the run like regular
function-objects.
The string is provided by a special class (the so called
dictionaryProvider). Current implementations for the provider are:
- fromFileDictionaryProvider
- reads the text from a dictionary file
- stdoutFromCommandProvider
- executes a program and takes the standard output as the dictionary text
- stdoutFromPythonScriptProvider
- executes a python-script and takes the stdout as the dictionary text
The string must be in the format o a regular OpenFOAM-dictionary
with an entry functions from which the functionObjects are
generated
This FO in the simpleFunctionObjects reads a number of fields
and updates their boundary conditions at every timestep.
Main purpose is to let groovyBC do calculations and use the
results for post-processing purposes
Does not support surface-fields as these don’t have a
correctBoundaryConditions-method.
Example of the usage in the angledDuctImplicit-case (the
results are of limited value because of the temperature boundary
condition)
Three source terms were added. These source terms are in the
swakSourceFields-library and can be used with solvers that use
the sourcesProperties-dictionary. The sources are
- SwakSetValue
- sets values according to a mask or the
mechanism provided by
basicSource - SwakExplicitSource
- Uses the calculated source term on the right hand side of the equation
- SwakImplicitSource
- Uses a calculated scalar-field to add an implicit source term (source is without the actual field)
These fields are only implemented in the 2.x-version of swak
because the interface of basicSource is very different in 1.7
and a backport was unnecessary
simpleFunctionObjects now has a function object
writeAndEndFieldRange that stops a run (and writes the last
time) if a field is outside a specified range.
A similar function object writeAndEndSwakExpression is in the
simpleSwakFunctionObjects that stops if a swak-expression
evaluates to true. writeAndEndPython does the same in
pythonIntegration.
Note: after the run is written one more timestep is calculated (this seems to be due to the fact that FOs are calculated at the start of a timestep). Also there are issues if the next timestep is a scheduled write-time (this only seem to be an issue with 1.7.x. It all works fine on 2.1.x)
New function objects in the simpleFunctionObjects allow the
loading of such models for solvers/utilities that don’t have such
models but where some functionObject (for instance) needs such a
model to be in memory
Added as part of the simpleFunctionObjects some functionObjects
that create a cloud of particles and evolve them at every
timestep.
The appropriate fields needed by every cloud have to be present
(either supplied by the solver or via a functionObject)
This function objects allows the manipulation of patch fields
like manipulateField allows the manipulation of the internal
field. Only use if desperate
If a variable is declared in the delayedVariables-list then its
behavior changes: when a value is assigned to that variable then
the value is not immediately used but after the time specified in
delay. Values are stored at intervals storeInterval and
interpolated linearly. If no stored data is available then the
value of the expression startupValue is used.
This feature allows the modeling of boundary conditions that react with a delay to flow conditions
To satisfy the requirements of certain boundary conditions
funkySetFields now allows the preloading of fields. This is
only available in dictionary mode with the preloadFields-entry
(for each entry in the expressions-list separately)
The environment variable SWAK4FOAM_SRC is needed for the
swakCoded-functionObject. The Allwmake-script now checks
whether this variable exists and prints a message with the
correct value if it doesn’t. It also checks whether the value is
correct and warns if it isn’t
The links to mybison and myflex are missing when the sources
are downloaded as a tarball. The Allwmake-script now creates
these links if they are missing
Sources of the parsers have been completely reformatted to make them more readable and maintainable
Make the directory a little bit cleaner
To avoid clashes with other similar efforts (not that I know of
any) the library libpythonIntegration.so has been renamed to
libswakPythonIntegration.so.
Usually only the libs-entry in the controlDict has to be
changed (if the library is used at all). Names of the function
objects stay the same
Now the outputControl-entry is honored. If set wrong the field
is no longer calculated/manipulated at every time-step
Branch only compiled on 2.1, but not on 2.0 due to changes in the OpenFOAM-API
Fix provided by Bruno Santos
If no refValue is given during construction then a value of
Fixed by using the value as the refValue if no refValue is
specified
The error message occured much later when a tmp tried to copy a
NULL-pointer and was not obvious at all for the general user. Fixed
1.6-ext does not consider the product of two symmetrical tensors to be symmetrical. Fixed
Change in the interface of the ExpressionResult-class
broke the access of global variables from a
Python-functionObject. Fixed
This didn’t influence the compilation (as there is already a current version file there) but confused people.
Face and point fields did not propagate the information correctly and were treated as non-uniform volume fields of the wrong size. This should now be fixed
The reason was that the patches of the divisor had a value of
zero. This has been fixed by only dividing the
internalFields(). Same for pointFields.
This kind of patch was not identified as something that could have the value fixed
The definition of the operator lessOp clashed with another
definition. Renamed.
Fix provided by Bruno Santos
expressionFields were calculated at every time-step, even if
the computational cost was high. Now if outputControl is
outputTime the field is only calculated if it is going to be
written
Seems like this one was overlooked because gcc is more
tolerant towards stupidity.
Reported by Edo Frederix
On the slides the case files were promised
It is now possible for expression on internalFields to access
fields from different cases. These fields are always read from
disk when being accessed for the first time and stay cached in
memory until the time is changed. The data is interpolated to the
current mesh with the meshToMesh-class (which is the workhorse
of the mapFields-utility)
The meshes are stored in a repository and are accessed via a
name. If for instance the mesh is known under the name
otherMesh then in an expression the term otherMesh(T) is the
field T from that other mesh at the specified time interpolated
to the current mesh.
Certain function objects and parser instances allow specifying
foreign meshes in a subdictionary foreignMeshes.
This is the long asked for feature to “get non-uniform values
from other patches”. It only works if the patches are specified
as mapped (or directMapped for 1.x). Therefor a patch can
only access one other patch with this.
On a mapped patch mapped(T) gets field T from whatever this
patch maps from (other patch, cells, faces). mappedInternal(T)
gets the values from the internal cells on the other patch (this
only works for patches).
On a mapped patch an external variable expression for patches now
changes its meaning: if other is the patch that the current
patch maps from (and only then) then var{patch'other}=expr
evaluates expr on the other patch and then maps the values to
the current patch (var may be non-uniform). In all other
circumstances var will get a uniform value which is derived
from whatever expr evaluates to.
To allow non-uniform offsets in the specification of mapped
patches in polyMesh/boundary a utility
calcNonUniformOffsetsForMapped was developed.
The framework for function objects that manipulate the runTime
were added. The concrete implementations are
- setDeltaTByTimeline
- set the timestep from a data file
- setDeltaTWithPython
- set the timestep by evaluating a Python-snipplet that should return a floating point number
- setEndTimeWithPython
- set the end time from the evaluation of a Python-snipplet
The library libswakChemistryModelFunctionPlugin adds the
possibility to calculate properties of the chemistry like
reaction rates, chemical timescale and released energy.
Currently only implemented for psiChemistryModel
If there is no chemistry model in memory it will be loaded and the reaction rates are calculated.
There is a function psiChem_updateChemistry that forces the
chemistry to be recalculated with a specified timestep. For
technical reasons this returns a scalar field with the value
psiChem_updateChemistry(0.0001)+psiChem_RR(CH4) calculates the
reaction rate assuming that the timestep is
Two additional functions that sum up all the reaction rates (this
should be
The library libswakRadiationModelFunctionPlugin adds the
possibility to calculate properties of the radiation like
parts of the source terms Rp and Ru and the current
radiation source
If there is no radiation model in memory it will be loaded and
the reaction rates are calculated. Assumes the presence of a
temperature field called T.
If the numpy-library is found then global variables which are
fields are being transformed to numpy-arrays. These arrays can
be accessed with the usual numpy-array access like a[i,j] or
a[i,:]. Global variables are made accessible by
reference. This means that writing a value changes the global
variable. Setting the whole variable has to be done by slicing
a[:]=3 (a=3 removes it from the workspace). Vectors and
tensors are two-dimensional arrays. They have
convenience-attributes that return the whole vector of a
component (like a.x for vectors or a.xx for tensors). To
overwrite these they have to be sliced: a.x[:]=0 (a.x=0 only
changes the attribute)
If a variable that is going to a global namespace is a
numpy-array then it is translated by the following rules:
vectors are transformed to scalarField. Arrays with 3 columns
to vectorField, 9 columns to tensorField and 6 columns to
symmTensorField. Different column-numbers produce errors
If this is set then this Python-code is executed every time a time-step was written to disk
Python-integration now has two convenience-functions that return a filename with the full path and create the directories if necessary. The file is not created (that is the responsibility of the Python-code).
The functions are (name is the name of the function object)
- dataFile(fname)
- creates a directory
<case>/<name>_data/<time>. To be used for data that is written at times that differ from write-time - timeDataFile(fname)
- creates a directory
<case>/<time>/<name>_data. Should only be used for data that is written only at write-time
A command lione switch -noDimensionChecking is added that
allows switching off the checking of dimensions if this makes
expressions fail
If another case (with time and region) is specified via command
line options (no dictionary) then in the expressions the other
mesh can be accessed under the name other
Main application for this is comparing to other cases (but also comparing different timesteps of the same case with each other).
Used time is either fixed or set to the currently used (this can be selected via the command line)
Each expression can specify foreign meshes with a
foreignMeshes-subdict
There are two new function objects:
- addForeignMeshes
- this allows specifying new foreign
meshes. These can be used in subsequent function-objects or
other swak-expressions on
internalFields - foreignMeshesFollowTime
- this allows specifying a list of meshes whose time is set to the current time of the running case
This helps debugging timestepping-strategies
A new possible entry for the accumulations calculates an
average that is weighted by a facetor that depends on the entity:
- cell volume if applicable
- face area for surfaces etc
-
$1$ if there is no appropriate weight (usually values defined on points). The result is equivalent toaverage.
The title says it all. Should give the user additional feedback about what is happening
This boundary allows specifying the partial slip fraction of the
regular partialSlip-BC with an expression.
This is sometimes necessary to allow calculations with fields where the boundary conditions have a lot of dependencies (turbulence model, other mesh etc)
The option -additionalRegions allows selecting additional mesh
regions for boundary conditions that require it (usually used
together with -preloadFields).
For the other case there is an additional option
-otherAdditionalRegions.
This option allows specifying additional field names to be preloaded in command line mode. If multiple mesh regions are specified (including another mesh)it will try to preload the field there too
Support for tensor-types has been added
For boundary conditions that require other fields these can be loaded into memory
The utility now allows the selection of timesteps. In that case it acts fundamentally different: instead of doing a timeloop it jumps to those times, calculates the boundary conditions and writes. The purpose of this mode is generating boundary fields for postprocessing.
As the majority of installation problems were actually problems
with the compilation of the library swak4FoamParsers and as
this library is central for all other things in swak4Foam the
compilation terminates if this library is not built
This new header includes information about the
swak4Foam-version, the OpenFOAM-version and macros for
workarounds that depend on the OpenFOAM-version
This forces the entries to be checked while being read. Allowing more consistent treatment
This script allows compiling additional versions of
swakPythonIntegration for cases where the version on the
development machine is different from the version on the
simulation machine (see installation chapter)
Changes without consequences for the user
The valid characters for an identifier were the same as in word
(was string before)
The list of contributors to each file have been added (mostly by script with the information from the repository)
This abomination from the early days of funkySetFields has been
cleaned
Changes to the documentation
A first version of a reference manual is added. Only the first part about expressions and parameters is written.
This is the first version to compile with OpenFOAM 2.2
Due to changes in OpenFOAM it requires several #ifdef (something
that is usually avoided in the OpenFOAM-world) and other
prepocessor definitions)
Due to incompatibilities between OpenFOAM 2.2 and previous versions there are compatibility headers included from the rest of swak4Foam.
Theoretically both libraries can be easily made independent again.
The last release (0.2.2) did not compile on 1.6-ext. This is
fixed
Due to a stupid .hgignore the 0.orig-directories were
missing. Nobody complained though
This has been fixed
With the options autoWriteSurface and autoWriteSets sampled
surfaces and sets are automatically written at each write
time. With writeSurfaceOnConstruction and
writeSetOnConstruction both are written when they are
created. A format has to be specified. No values are written.
These function and some other minor ones (sph, dev2,
twoSymm) are now supported by the parsers
The component operators .x, .y and .z now extract the rows
from a tensor
As this situation (like a variable named p for the position
that shadows the pressure field p) leads to weird errors a
warning is given. The warning can be switched of with the option
variableNameIdenticalToField.
According to the convention introduced in OpenFOAM 2.2 now the
data directories generated by functionObjects based on
simpleFunctionObjects (that is almost all) and
swakPythonIntegration (if the Python-code uses the
dataFile-function) are generated as sub-directories of
postProcessing in the case directory.
Scripts that rely on the location of these files will have to be adapted
This is due to a fix that now allows reading/writing these in binary mode. Only occurs if reading old data that either
- uses a delayed variable
- has global variables written in timesteps
This may break them for previous versions of OpenFOAM
The C-files generated by bison become very big and some
compilers need quite long when aggressive optimization is
used. An additional environment variable
SWAK_COMPILE_GRAMMAR_OPTION allows the specification of
additional compiler switches (like -O1) that will appear
after the regular switches and should alter the behavior of
the compiler. Set in swakConfiguration if you want to set this
permanently
Some distributions don’t use good old bash as the default
shell. This breaks some scripts in subtle and not so subtle ways
To filter bug-reports with outdated versions
Changes without consequences for the user
Methods that look for fields now use the appropriate data type
There were template specializations for pTraits in
ExpressionResult.C that had to be moved to ExpressionResult.H
to allow compilation on these non-=gcc=-compilers
Even if the condition evaluates to false the function objects
in the list are executed. This makes the run fail if the purpose
of the condition was to guard from such a situation. Fixed
This was fixed by writing the fields properly with
writeValue. This may introduce a little incompatibility when
reading files written by old versions
These fields were registered with the mesh which might have disturbed similar named real fields. Also did the fields generated for variables get registered
Missing initial conditions made this case a bit pointless
This was due to the boundaries being set to 0. Fixed. Also for
the dist() function
The library simpleSearchableSurfaces adds more searchable
surfaces to be used in snappyHexMesh. Types of surfaces in
that library are
- some objects that duplicate existing surfaces and are only there for historical reasons (except the cylinder which distinguishes between different sides). Others wrap existing surfaces and expose the different sides
- wrappers for other surfaces that do coordinate transformations with it: rotation, translation, scaling
- wrappers that take two surfaces and do boolean operations with them: union, intersection, difference, exclusive difference
- Some wrappers that manipulate the regions of a surface: rename them, collect them into one region
This type is used to collect multiple values. If it is assigned a value then the uniform value of the right hand side is appended to the variable. Useful for collecting multiple values for output.
Variant StoredStackExpresionResult keeps the values between
timesteps and allows the collection of timeline data
Dumps the value of a global variable into a line of a file
Removes a global variable (mainly used to preserve memory)
This dictionary allows the specification of alias names and
their real names. If an alias name is found in an expression
then it is replaced by the real name when looking for
fields. The application for this is that OpenFOAM allows
characters in field names that are not valid in swak-names and
would break the grammar if they were (for instance - or
:). By setting an alias such fields can still be accessed.
The function object listRegisteredObjects in the
simpleFunctionObjects lists all the objects currently
registered with the mesh. Mainly used for debugging (“Which
fields are currently available?”)
The new functionObject executeIfParallelSerial allows
specifying if a list of function objects should only be run if
the simulation is running in serial or parallel.
There are now four function objects that calculate distributions
of fields. Distributions are calculated based on the
Distribution-class that is part of OpenFOAM starting from
version 2.0 and uses a weighting for added values. There are two
kinds of output
- a timeline with the key characteristics of the distribution
- directories with the distributions at specific times. These are written “raw” and accumulated
For tensors and vectors these are output separately for every component. These outputs can be switched on and off separately. The user has to specify the bin-width for the classification. If the bin-width is too small and the distribution becomes too small it is scaled down.
The two function-objects in the simpleFunctionObjects are:
- fieldDistribution
- distribution of field values weighted by the cell volume
- patchFieldDistribution
- distribution of a field on a number of patches weighted by the face area
In swakSimpleFunctionObjects the two functionObjects are:
- swakExpressionDistribution
- distribution of an
expressionon some entity. The user also has to specify and expressionweightwith the weight of each value and a logical expressionmask. Values are only used ifmaskistrueat the place - patchExpressionDistribution
- distribution of
expressionon a number of patches. As the weight the face-area is used
This allows other variable types like stored variables to be inserted there. They are also now saved for restarting
All classes using the python interpreter now have a variable
endTime with the current end-time value
If one of the functionObjects for time-manipulation set the end-time and it is reached and this is no time for output a complete output of the fields is forced
This includes the patchExpression-functionObject. The supplied
list is now interpreted as a list of regular expressions and all
patches that match are included and processed
An optional parameter outputControlMode now allows control on
when the function object will be executed. Possible values are:
- timestep
- Every
outputIntervaltimesteps the object will be executed. This is the default behaviour with an interval $1$ - deltaT
- Approximately every
outputDeltaTtimes it will be executed. The nearest possible timestep is used - outputTime
- Executed whenever a regular output is scheduled
Two enhancements
- the name of the independent variable no can be specified. This variable holds the value that is passed to the data entry as a uniform value
- data entry can now be integrated. This allows using it for instance for the injection rate in lagrangian models
The reason for the jump in the minor revision number is that with
the introduction of the parser for lagrangian particles (cloud)
the last white spot as far as major data structures in OpenFOAM is
“explored”
Due to certain differences this version only compiles with the
nextRelease-branch of 1.6-ext (from the git).Usually the
failing parts can be fixed b commenting out the appropriate
#define in Libraries/swak4FoamParsers/include/swak.H.
As this version is quite similar to 1.7 a lot of #ifdefs were
introduced by this port leading to a possible unification with
the 1.x-branch
The error messages where already quite verbose. But people didn’t understand them and asked the same questions over and over …
As there are going to be more cross-dependencies the
simpleFunctionObjects now have to be part of swak. Changes to
the compile-scripts reflect this.
The script writes the version it is used with to disk and at later compiles that this is the same (this makes sure that not a wrong version is used inadvertently to compile)
There are two macros defined that inside an object write the name of the class and the address of the object (if debug is enabled). This makes the output easier distinguishable from the output from other classes/objects. The two macros are:
- Dbug
- Writes the debug information only on the master processor
- Pbug
- Writes the output on all processors and for parallel runs prefixes the processor number
Both macros are to be used like regular streams and don’t have
to be enclosed in if(debug){} (this is part of the macro)
With some compilers (Intel) and aggressive optimization the
lexers (whose code is generated by flex) have uninitialized
memory and segmentation faults. In these cases now an environment
variable SWAK_COMPILE_LEXER_OPTION to set lower optimization
for these compilers. For example:
export SWAK_COMPILE_LEXER_OPTION=-O0
After that recompile
For some machines race conditions with compiling the main library has been reported. The reason seems to be that some source files need headers generated while compiling the grammar. If due to the large number of simultaneous compilation processes the headers have not been generated when these files are compiled the compilation fails.
This effect could not be reproduced on the development machine (but that doesn’t mean that this doesn’t happen on some machines). Nevertheless for the libraries where this might be the case the number of compilation jobs is limited to the number grammars in the library.
Better solution to let the Allwmake-script generate the headers
before the regular wmake starts.
Several minor additions that should make packaging easier
- Package version now gets the correct distro name (at least on Ubuntu)
- Packaging picks up the correct python-version (2.7 or 2.6 … does anyone use older?)
- Packaging process leaves the
swakVersion.Halone
Important enhancements of the documentation in the
Documentations-folder
The possible values of the common accumulations-lists are
documented
The general options and the behavior of the Python-embedding are described
Because of report https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=177 to be consistent with the nomenclature in the ‘regular’ function-objects.
This method has been added in 2.2.x and breaks the compilation of several function-objects
Fix developed by Bruno Santos
For some reason using SuSp gave unstable results for the
PDE-functionObjects. Changed to Sp
Bug originally reported https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=179 in. Reason was that the variable describing the type was not correctly set.
The entries codeEnd and codeExecute were not correctly read
but instead the entry codeRead was read. Fixed
Reported as https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=172
Only the field parser correctly found logical variables (although
they were stored). Added a method to pick up the variables (the
reason why this part was commented out is that there is no such
thing as a volBoolField and that is what the regular mechanism
expected)
Reported as https://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=176
In that case the driver was written before the surface was
updated thus generating fields of size update is
called at various places (to make sure it is called in any instance)
This accumulation was available but not implemented. Now implemented.
For non-scalar types it is calculated separately for each component
This was due to a logical error that was propagated through mindless copy/paste (only the Field-driver got it right). Fixed
Because it is not initialized from the superclass when the dictionary constructor is used. Fixed
Because the pointer is already set. Fixed
If the dictionary was read after the construction the aliases are not read. Fixed by moving this reading to the tables reading which is used in every time a dictionary is involved
Passed a value where a reference would have been needed. Fixed
Reason for this was a change of the interface of outputTime not
being propagated to this function-object. Fixed
The Python-integration returned single scalars (and vectors) not
as a single value but as a field of length
These were not compiled by accident. Fixed
As reported in http://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=190 if a face-set or zone has faces on a processor boundary incorrect values were produced.
The reason was that boundary faces are treated like internal faces. Also do these faces exist on both processors. This is now fixed. If the face is on a regular boundary patch the value is used. If on a processor patch the value is only used if it is on the owner processor.
This addresses http://sourceforge.net/apps/mantisbt/openfoam-extend/view.php?id=190
Subclasses of simpleFunction-objects are not guaranteed to be
parallel-aware (for instance swakExpression can have problems
with stored variables if the number of cells/faces changes) so
the notImplemented can’t be removed for good.
The workaround is a rather verbose error message and the
possibility to override notImplemented with a dictionary-switch
The functionObject executeIfOpenFOAMVersionBiggerEqual only
executes if the OpenFOAM-version is bigger or equal to a
specified version. The arguments majorVersion and
minorVersion are required. If patchVersion is not specified
it will match any version. A git version (.x) will match any
patch-version
The function object executeIfStartTime executes its children
if the current time is the startTime from the controlDict
(which isn’t necessarily the first time step in a restarted case)
To be used on an existing field to set reasonable initial conditions
Named recalcPhi in the simpleFunctionObjects. Usually needed
when some other functionObject manipulates velocity or density
Name correctThermo. Recalculates the thermophysical
model. To be used after manipulating temperature etc
Recalculate enthalpy, sensible enthalpy or internal energy according to the current temperature. This allows making this consistent if the temperature has been manipulated.
For OpenFOAM after 2.2 these are replaced by one that recalculates the energy or enthalpy
The function object swakExpressionAverageDistribution
calculates the average of one function (the expression) as a
distribution over another (the abscissa). An example would be
the average pressure in x-direction with abscissa being
pos().x, expression being just p and the weight
being vol(). The weight has to be a scalar. All other
expressions can be any data-type
This utility prints some quantitative statistics about a specified field. Optionally these statistics can also be printed for patches, sets and zones. The data can be written to a CSV-file. Also the distributions of the field can be written.
This utility needs a dictionary and a specification of times. For each time it
- loads a list of fields specified in the dictionary
- executes a list of function objects specified in the dictionary
- executes python-scripts
The idea is that the function objects pass data to the python-scripts via global variables and the python-scripts do whatever they like
This utility allows setting new fields of a lagrangian
cloud. Like funkySetFields it has two modes:
- Setting one field over the command line. This is triggered by
the
-field-option - Using a dictionary to specify what is being set. In this mode more than one field and more than one cloud can be set. In this mode there is also the possibility to specify a new cloud. This mode expects variables in global namespaces. On of these variables is the position of the particles, for the other variables fields of the same name will be created. All the variables have to be of the same size. Data where corresponding particle position is outside the mesh is discarded
There is now an additional parser to calculate expressions on particles.
This parser is organized in a separate library
libswakLagrangianParser that has to be loaded to use this
parser.
Depending on whether the cloud in question is already in memory or on disk the data is handled differently:
- if the data is on disc then the basic properties of the cloud
(particle positions etc) are used to initialize the class. Then
all files in the folder of the cloud are read and made
available as field names that are the same as the
file-names. Characters in the file names that are not
compatible with the parser are replaced and created as
aliases. In this mode
swakhas no idea about the data except the name and the type - if the cloud is in memory then a corresponding proxy object is
sought. This proxy object knows which data the cloud has, what
the type is and a short description. It makes the data
available as fields.
swakhas by default proxy objects for most particle classes that come withOpenFOAM. For unsupported classes and adaptor library has to be written.
When a parser for a cloud is used for the first time a table of all the available fields is printed to the screen with type and description (if available)
If the field is found in memory this is used instead of a file read from disc.
An additional switch writeBeforeAfter allows writing the field
before and after solving
Mode startup executes the FO only during construction
It is now possible to add a sub-dictionary else that is used
to initialize a functionObjectProxy that is executed if the
condition is not fulfilled. The sub-dictionary inherits all
settings that are not set from the parent-dictionary
The entry codeData is now read and inserted into the functionObject
The two parsers in that library now also support the complete
set of tensor operations (like eigenValues etc)
For expressions whose results is not a scalar now the weight function can either be a scalar or of the same type as the expression (so every component can have a separate weight)
A number of possible accumulations have been added. Most of
these are based on distributions. If the weighted variant is
chosen then the meaning is the more physical one (for weighted
the ‘natural’ weight of the quantity is used. For instance for
cells the cell volume. Otherwise the weight
- weightedSum
- sum of the quantity times the weight. There is
an alias
integratefor this - median
- The value for which 50% of the distribution are
smaller than this. More robust alternative to
average - quantile
quantile0.25for instance is the value for which 25% of the distribution are smaller than it- range
- The difference of the quantile of $\frac{1+f}{2}$ and
$\frac{1-f}{2}$. For instance
range0.9gives the range in which 90% of the values are (from the quantile 5% to 95%) - smaller
- The fraction of the distribution that is smaller than a given value
- bigger
- The inverse of
smaller - size
- The size of the underlying entity (usually number of cells, faces, points). For types with more than one components all the components have the same value
- weightSum
- Sum of the weights of the underlying entity. Usually the volume oder the area of it.
If a file specified with an option like startFile in a
Python-functionObject (or similar) is not found in the current
directory the path of the dictionary it is specified in is
prepended and the file is searched there
The interactive shell of the python integration now uses
IPython if it is installed. This improves tab-completion etc
As problematic libraries could hand during importing these
libraries can be imported in a safe way using the optional
importLibs-entry which is a dictionary. The keys are the names
under which the imports will appear in the Python-namespace. The
value is optional and the name of the actual library
All parsers now implement a function weight() that returns the
“natural” weight that is used for instance in the weighted
average (for internal fields that would be for instance the cell
volume)
Two kinds of files are optionally written
- CSV-files with the values of an evaluation (each evaluation gets its own file)
- Distributions of the evaluations (in a separate directory for each time)
All the files go into a directory whose name is derived from the
name of the evaluation. The outputs can be switched on with the
options writeDistributions and writeCsv. Either
- from the command line: this switches it on for all evaluations
- one “per dictionary”-basis for each evaluation separately
The PDE-functionObjects now honor the relaxationFactors. If
=steady is false then relaxation has to be switched on using
relaxUnsteady. For the last corrector iteration the equation
is not relaxed unless the parameter relaxLastIteration is set.
The support of laplacian operations (especially with a
coefficient that is different from a scalar) was incomplete. Now
all possible coefficient types are supported.
Also in the fvcSchemes-plugin functions the set of
laplacian-operators was completed
If the logical expression mask is set then only the results
from expression for which mask is true are used for
accumulations
Started one new directory for all cases from presentations
Two new examples
- sandPitsOfCarcoon
- Reenacting a scene from “Return of the
Jedi” with
twoPhaseEulerFoam - landspeedersInCanyon
- Simulating two landspeeders from “A new
hope” with
simpleFoam
There is now a new code-snipplet required for a number of these function objects. It can be left empty but has to be specified
The expressions used with swakExplicitSource,
swakImplicitSource and swakSetValue now also need a
dimension. This dimension is used to make sure that the user
“knows” the actual dimensions of his source terms
This version adds support for OpenFOAM 2.3. The major changes were due to changes in the API to
searchableSurfacemeshToMesh
And several minor adaptions
No major changes required. Runtime-selection tables are now sorted too
This should make swak.H more readable
If a directory privateRequirements/bin is private in the
sources directory then the bison found there is used. A script
maintainanceScripts/compileRequirements.sh is provided that
fetches the bison sources, compiles them and installs them there
A section about thus new feature is added
The distribution data was not clipped to the range where actually
data was collected. This is now fixed by adding the notion of an
invalid value to SimpleDistribution
This should now be fixed
Because of the missing dimensions until now swakExplicitSource
and swakImplicitSource were not actually working
Always set source etc for whole region. Now the selectionMode
is honored (for instance only in cellZone the source term will
be applied.)
Problem is that when the processor boundaries are used too that the indexing might be inconsistent on the different processors. Fix: coupled boundaries are ignored by default (have to be switched on)
In newer version the execute()-method of function objects
needs a parameter force. Fixed
Due to a small semantic difference in the copy constructor of
GeometricField a temporary object of the same name shadows the
real field and prohibits that it is written. Fixed by giving the
copy a unique name
These boundary conditions allow specifying a value in normal
direction to the patch while in tangential direction the regular
slip condition is applied. This is implemented for fvPatch and
pointPatch. For the pointPatch the normal direction has to be
specified by the user
Utility that calculates new point values for the mesh. In the
simplest form the expression is specified on the command line. If
the option -expression is missing the program looks for a
dictionary which allows more control. If -relative is specified
points are moved by the result of the expression. The result of
the expression must be a pointVectorField
A hierarchy of function objects that trigger additional writes. Once a condition is fulfilled data is either written for a specified interval or as long as the condition is fulfilled. After that a cooldown period is possible. During this period nothing is written.
The concrete function objects are
- writeIfFieldOutside
- writing is triggered if the minimum or
the maximum of a field is outside a specified range. Part of
the simpleFunctionObjects
- writeIfSwakExpression
- writing is triggered if a logical
expression evaluates to
true. Stopping and retriggering is also possible with logical expressions. Part of thesimpleSwakFunctionObjects - writeIfPython
- writing is triggered by a Python-snipplet that
either returns
TrueorFalse. Stopping and retriggering are also possible. Part ofswakPythonIntegration
Allows saving and writing a specifiable number of timesteps before the condition is met (this allows finding out what lead to this)
This function object installs a new signal handler for specified signals.
The function object itself saves the last
Starting with OpenFOAM 2.2 (where the concept of fvOptions was
introduced) there is an additional library swakFvOptions with
special fvOptions (in addition to those in swakSourceFields):
- executeFunctionObjectsFvOption
- this one does not manipulate the fields (as expected) but “only” runs a list of function objects. Application is for instance to get information during the time-step for algorithms that have multiple iterations in a time-step
- reportAvailableFvOptions
- Does no manipulation of the
solution/equations. Simply reports that a callback has been
called. Application: find out which
fvOption-calls are used by a solver in which order without going through the sources - reportMatrix
- Does not manipulate the matrix but prints a number of metrics
For expressions and variable lists there is now the possibility to expand values from the dictionary during reading. The two characters that trigger this are
- $
- like the regular variable lookup in OpenFOAM.In its most
complex form it looks like this
$[(type)spec]wherespecspecifies where to look for the value (including scoping if the OpenFOAM-version supports it). The optionaltypespecifies how the entry should be interpreted - #
- in variable lists:
#otherList;includes the variable listotherListinstead of this entry
These expansions allow the construction of reusable snipplets that include information from other parts of the case. For instance (this is only part of the specification)
#include "$FOAM_CASE/constant/g"
vecName U;
downComponent (
"grav=$[(dimensionedVector)g];"
"down=($vecName & grav)/mag(grav);"
);
variables (
"#downComponent;"
"maxDown=max(mag(down));"
);
would calculate the component of a vector field that points in
the direction of the gravity (as specified in the g-file).
This expansion is done during the expression.
An optional entry dimension for the function object now allows
setting the dimension of the resulting field
This function gives the distance in the mesh to a specified face.
Not yet working correctly
With the switch storeAndWritePreviousState this functionObject
now can cache a number of timesteps and write these results in
addition to the current timestep
In addition to the average now this Function object also records the minimum and maximum value for each bin. Also the number of samples used in the bin
The function objects executeIfPython, setDeltaTWithPython,
setEntTimeWithPython and writeAndEndWithPython now expect
code snipplet named init. This is executed in the beginning and
can be used to set up global variables if these snipplets need
some kind of state. The variables have to be declared global in
the snipplets that do the actual decision (for technical reason)
The function objects solveTransportPDE and solveLaplacianPDE
now call the regular fvOptions-callbacks (this allows modifying
the solution in the same way it can be modified for solvers)
Example to demonstrate funkyWarpMesh and post-processing on
bended geometries
This is the last release to support OpenFOAM 1.7.x and older
These are things that will happen in the next release and will break backwards-compatibility
As version 1.7 is several years old this release will be the
last release that supports it.
Starting with this release the port_2.x-branch will become the
default branch and the 1.x will become legacy
Due to the umber of different supported Foam-versions not all the
examples run on all versions and it is not possible to fix them
in such a way that they work on all versions. In the next version
they will by adapted to use the pyFoamPrepareCase.py utility as
this supports having different Foam versions in one case. As a
consequence most cases won’t run without an installed PyFoam
If value is unset then during initialization the value of the
internal field next to the patch is used. Previous behavior was
to set the patch to
In most cases the new behavior should be better.
As OpenFOAM does not support geometric fields of type boolean
swak uses scalar fields for storing truth values (only in the
internalField-parser). The semantics was that a value of 0
means false. Everything else true. Logical operators set
true to false to true. All others as false.
If operators were used properly this should not matter, but
expressions that assume for instance that 0.1 is true will
now fail. Overall this change improves the stability of logival
expressions
The improved detection of single values might break some expressions. Especially for the Python-integration as values that were previously passed as arrays are now being passed as single values
This reflects a change in the API of the kinematic lagrangian parcels. The old function has been discontinued to avoid confusions with changed semantics
For parallel runs this signal is now automatically switched in so that other signals are propagated to other processors
Due to a different calculation automatically calculated bin-widths in this function object might slightly differ from previous calculations
For the swak-function objects the data is now written to a
directory whose name is based on the input dictionary instead of
postProcessing.
This might break scripts and other post-processing procedures
that rely on the data being in postProcessing.
Data generated during the run-time of the solver is unaffected
Only minor adaptions. Mainly to accommodate the new debug switches
Compiles with OpenFOAM 2.4.0 (and 2.4.x)
Results that were booleans used to report bool as their type
for the internalField-parser. Now they report
volLogicalField, surfaceLogicalField or
pointLogicalField. This makes them consistent with the
possibility of requesting these start symbols and specifying
logical fields in the parameters of a plugin function
If the span of the abscissa is too small (almost
Reason was that SimpleDistribution.calcScalarWeight did not
reduce. This is now fixed (and a special switch is introduced
for one situation where this isn’t desirable)
On OpenFOAM-versions with fvOptions these were broken because
of inconsistent dimensions.
This is fixed: now if a fvOption is defined the
function-objects also needs rho and this is passed to the call
of fvOption when generating the source term
As reported in https://sourceforge.net/p/openfoam-extend/ticketsswak4foam/225/
Problem seems to be that the HashPtrTable is not correctly read
in binary-mode. Workaround is to switch to ascii before
writing and reading that table and then switch back to the
original mode
Single values like min(expr) were passed as arrays instead of a
single value. This is now fixed. The problem is that now
expressions that rely on the old behavior might break
If all data falls into one bin of the distribution then the distribution was not written. This is now fixed
Fixed
If the current time was already written (because it is part of the stored times) a segmentation fault occurred. This has been fixed by checking whether the current time is already stored
This has been fixed
The scripts
makeSwakVersionFile.pymakeCopyrightEntries.py
have been adapted so that they now work with Python 2.x as well as Python 3
This function for the field parser gives the distance in the mesh to a specified patch. Distance is defined as minimial sum of cell-to-face distances needed to reach this cell from the named patch
If a SIGSEGV or SIGFPE were encountered only on some
processors then on the others no data was written because these
signals do not propagate to other processors
Now the signal handler raises a SIGTERM which is propagated to
the other processors. For parallel runs a signal handler for
SIGTERM is automatically set up to make sure that on all
remaining processors data is written
Provided by Alexey Matveichev
The script maintainanceScripts/make-releases.sh rolls a release
and puts it into the directory releases
Provided by Alexey Matveichev
Automatically finds the linking options for Python with
python-config
Similar to distToPatch there are now two additional built-in
functions:
- distToCells
- A logical field is provided. The distance to the
cells for which this field is
trueis calculated - distToFaces
- Same as
distToCellsbut with a logical function for the faces
Both functions return cell-values
This library collects functions that are similar to
distFromPath: they use the MeshWave-algorithm to calculate
distances and connectivity of the mesh.
Functions in this plugin are:
- meshLayersFromPatch
- Calculates for each cell how many mesh layers it is away from a patch
- meshLayersFromCells
- Calculates the number of layers from a set of cells selected by a logical expression
- meshLayersFromFaces
- Calculates the number of layers from a set of faces selected by a logical expression
- floodFillFromCells
- Number connected regions. Cells selected by a logical expression separate these regions
- floodFillFromFaces
- Number connected regions. Faces selected by a logical expression separate these regions
- cellColouring
- “Colors” the cells in such a way that no two neighboring cells have the same number. Mainly for visualizing the mesh structure. “Neighboring” means “cells sharing a face” not an edge. Therefor it may look at the surface like there are cells with the same color
Additional functions:
- mqCellFaceNr
- Number of faces for each cell
- mqCellShape
- Field with numbers describing the cell
shape. Values are:
- 1
- Hex
- 2
- Prism
- 3
- Wedge
- 4
- Pyramid
- 5
- Tetraeder wedge
- 6
- Tetraeder
- 0
- no classification. Polygon
The function object provokeSignal can be used to debug signal
handling. No other possible use is known.
The function object allows defining the signal, the time and - in case of parallel runs - the processors on which the signal should be raised
This function object executes a lost of function objects if
face/cell/point sets or zones are present. The required zones and
sets are specified in a dictionary setsAndZones: keys are the
names of the entities the values are the types (like
faceZone). Only if all objects specified there are present
the function objects are executed.
As a side effect if loadAndCacheMissingSets is true than sets
that are not yet found in memory are loaded from
disk. Attention: if no set of that name is found on disk then
it is searched at every time-step. This is a potential
performance problem (it is not a problem if the set is there)
This function object executes a lost of function objects if a list of patches is present.
This function object shows data that is stored in the
mesh. Mostly solverPerformance with the residuals of the linear
solvers
This function object gets a list of fieldNames and gets the
information about their solver performances. The three quantities
that it gets are
nIterations- the number of iterations
initialResidual- residual before iterating
finalResidual- residual after iterating
For each value three variables are created (assuming the field is
named foo):
foo_nIterations- array with all the values. This is usually only usable in the Python-integration
foo_nIterations_first- value of the first solver performance
foo_nIterations_last- value of the first solver performance
simpleFunctionObjects now has a base class that allows
manipulating fvSolution and fvSchemes in-memory but the
solver behaves as if the file changed on disk. Application for
this is changing parameters like relaxation or discretization
schemes during the simulation. This can be used for instance to
start the simulation with ‘safe’ settings and switch to faster
convergence later.
There is currently only one function object
timeDependentFvSolutionFvSchemes that implements this (more are
planned). It allows switching to different subdictionaries at
specified time. An example can be found at
Examples/manipulateFvSolutionFvSchemes/pitzDailyTimeSwitched.
This function object gets a list of times and
sub-dictionaries. At the specified time the values from the
sub-dictionary overrides the values in the original dictionary
(Values not present in the sub-dictionary are left untouched). If
reset is specified as the name for the sub-dictionary then the
dictionary is set back to the original state.
Until no if value was not set groovyBC automatically
initialized the boundary to T to
Now if value is unset then the value of the patch is
initialized from the value of the internal field next to the
patch. This doesn’t protect from the internal field being
With an additional optional argument cloudNames a list of
clouds to be written can be specified like the fields.
This feature was implemented by E. David Huckaby
For utilities for which this is appropriate this allows loading
function plugins from the command line (without adding them to
the libs-entry in the controlDict). It is assumed that the
name of the library starts with libswak and ends with
FunctionPlugin.so.
If a list of words named functionPlugins is found then the
string libswak is added in front and FunctionPlugin.so is
added at the end and a library of that name is loaded to add the
functions provided there
Now it is possible to handle SIGUSR1, SIGUSR2 and
SIGTERM. Only needed for testing
If a code is a string of the length
If a dictionary specifies the entries mask and weight then
these are evaluated and used to mask and weight the data
specified in expression
If specified in the sub-dictionary the entries
distributionMaxBinNr and distributionBinWidth allow setting
the number of bins. These values are not used exactly but give
the distribution class a hint. distributionMaxBinNr takes
precedence
For parallel runs the process that initiates the writing of data
waits for the other processes to write their data. This time can
be specified with a parameter sleepSecondsBeforeReraising that
has a default value 60
The function objects based on writeAndEnd now have an optional
switch storeAndWritePreviousState. If this is set then a number
of old time-steps can be stored and will be written when the run
is terminated.
In 2.3.1 two new forms of addSup where added to fvOption (one
for compressible equations. The other one for multi-phase
solvers). Both new forms are supported by all
fvOption-subclasses in swakSourceFields and swakFvOptions
When the switch dynamicExtremesAbscissa is false then the
limits of the distribution can be set with minAbscissa and
maxAbscissa. This mainly influences the bin-width. If values
fall outside this range then the distribution is extended to
accommodate these values
Function objects derived from simpleDataFunctionObject now can write to a different directory than postProcessing
This involves almost all function objects in swak that write data
to postProcessing. The library now allows setting a different
default. This value can also be set with an optional entry
postProcDir on a per-function-object basis.
This change is used in the funkyPythonPostProc-utility to set a
directory name that is based on the name of the input dictionary
(or set with an option). Now if there are function objects used
they will write their data to this directory instead of
postProcessing (leaving data generated during the running of
the solver alone)
Note: This only works for function objects from swak. “Regular”
function objects will still write to postProcessing
An additional option -correctResultBoundaryFields corrects the
boundary conditions before writing to disk. In dictionary mode
there is also an option correctResultBoundaryFields.
This is only needed in rare cases.
This case demonstrates how to add lagrangian particles to the simplest tutorial-case
This is the first release that does not support OpenFOAM 1.7.x, OpenFOAM 1.6-ext and older versions anymore
This version adds support for OpenFOAM-dev published at
git://github.com/OpenFOAM/OpenFOAM-dev.git
As this version is constantly changing it might or might not work with the most up-to-date version of the repository.
The port is maintained in a branch feature/port_of-dev that is
never closed and is periodically merged to the develop-branch.
Internally the dev-version is maintained as version 9.9.99
Support for this version has been added (basically all the fixes
from the dev-branch were guarded with the correct version
This version is supported by swak4Foam (compiles and runs)
This version is supported. For the time being it can be assumed that this version is similar to the regular OpenFOAM 3.0
Fields that have names that are not considered proper variable
names by swak (because for instance the have a dot in the name
like alpha.water) were not handled by fieldReport. This has
been fixed
The reason is the initialization with pTraits::max and that
during the calculation of mag this causes an overlflow. Fixed
by scaling down to the square root of the maximum
Because of this compilation in 2.2 failed. Fix provided by Bruno Santos
The reason was that the solverPerformance-class is hidden in
lduMatrix. Fix provided by Bruno Santos
For OF-versions where fluidThermo and solidThermo have the
same base functions like thermo_Cp can be used for solids too
Because of a bug in the lexer lookup tables did not work. Fixed
The macro that guarded the code needed for some OpenFOAM-versions did not include OpenFOAM 3.0. Fixed
The wrong flags were checked and the function objects were always
executed when even if doMakeAbsolute and doMakeRelative were
set to false. Fixed
A reference to a label that was passed to a flex-function
broke compilation because that expects a 32-bit integer. Fixed
Due to a copy/past-problem all tensor-fields (including symmtrical and spherical) would have caused the utility to fail. Fixed
The function object ignored the callbacks for moving meshes. It now implements them and forces a regeneration of the surface if the mesh moves
The dimension-entries were read but not set. This is now fixed
The utility now reads the compression state of the original and sets the resulting file accordingly
Point fields were not correctly returned. This is fixed
New version of org-mode makes changes in the UML-code necessary
Like the optional list lookuptables it is now possible to have
a list lookuptables2D with 2-dimensional lookup tables. A table
with the name tbl can be used like this in expressions:
tbl(expr1,expr2). expr1 and expr2 must evaluate to scalar
values of the same entity (cells, faces, points …) and the
expression will evaluate to a scalar.
This feature is based on the interpolation2DTable that is part
of OpenFOAM since 2.2 but there is a modified version of this
class included in swak4Foam as there is a problem with the
output in the original version. Currently foam-extend is not
supported as this is missing some base classes as well
(tableReader)
The Plugin DynamicMesh adds functions to visualize the mesh
movement. The functions are
- dyM_meshPhi
- the mesh
phias stored with the mesh. Some distributions write this field anyway - dyM_meshCourant
- Mesh courant number. Replicates the number some solvers print automatically
- dyM_meshVelocity
- Velocity with which the cells are
moved. Reconstructed from the mesh
phi
These functions might failed if the mesh has not been moved yet
so their calls might have to be encapsulated in a
executeIfStartTime function Object
The function object loadTopoSets loads all the available sets
in the mesh into memory for expressions that need them. Also
allows automatic writing of these sets (switched by writeSets)
The function objects manipulateCellSet, manipulateFaceSet and
manipulatePointSet allow the manipulation of these
topoSet. They do so by evaluating an expression mask and all
cells (faces, points) for which the expression is true will be
part of the topoSet. If the topoSet is not present in memory the
function object fails unless the parameter createMissing is set
to true. The entry writeManipulated (default: true) says
whether the topoSet should be written at write times.
An example of this functionality is found in Examples/other/topoSetDamBreak
The function object executeIfWriteTime in the
simpleFunctionObjects executes a list of other function objects
only if the current time is a scheduled write time. The purpose
of this function object is to only execute function objects at
write times that don’t honor the
outputControlMode-setting. Also does the else-branch allow
executing only when nothing is written
This function plugin makes a number of function from the
MRF-model available:
- functions to make fields absolute or relative in the
MRFregion - a function to calculate the Coriolis force
All these functions call the MRF-model
These function objects can be added to particle clouds. In this first version these objects can be added:
- cloudMoveStatistics
- Records simple statistics about the
solution of the cloud:
- How often were faces hit by particles (total, per particle: minimum, mean and average)
- How often were particles moved (same data as face hits)
- How often was each patch hit
Only minimum effort has been spent to consolidate this data across processors (particles may be counted on multiple processors).
The main purpose of this function object is to spot problematic behavior (particles that hit patches repeatedly and don’t move)
The optional parameter
reportHitNrandreportMoveNrprint out the ids of particles that exceed these thresholds - eliminateCaughtParticles
- Sometimes particles get caught in
“endless loops” (hitting the same patch over and over again
without significant movement). This may slow down
simulations significantly as basically the same impact is
calculated over and over again without any progress. Two
parameters allow eliminating such parcels:
- maximumNumberOfHits
- if the same boundary face is hit more often than this by the particle (without hitting any other faces) then the particle is eliminated. Recommended value: 1000
- minDistanceMove
- Minimum distance a particle has to move when hitting a boundary face. If it moved less the particle is removed. Recommended: $10-9$
If one of the parameters is set to a negative value the criterion is “switched off”
- eliminateOutsideParticles
- Removes particles that are outside the mesh (are not inside any cell). The purpose of this is to eliminate particles that are for some reason not correctly tracked
- correctParticleCell
- Correct the cell of the particle before
the evolution begins.
This should fix problems with moving meshes but is currently not working correctly.
An optional parameter
logCorrectedlogs the data of the corrected particles to a file. Only use for debugging or if you don’t expect many incidents - traceParticles
- This function object gets a list of particle
ids. For these particles all data is written whenever a
function object is called.
This function object should only be used for debugging if the behavior of a special particle should be tracked
These function objects can be added to particle clouds and use expressions. The function objects are
- eliminateBySwakExpression
- Evaluates an expression for each
particle. If the expression is
truethen the particle is eliminated. Expression can be evaluated before or after the moving of the particles
A function that calculates the stream function in a 2D simulation has been added
These functions from fvc were implemented as
plugin-functions. Mainly to be able to test their behavior. To
check what they do see fvcSmooth.H in finiteVolume
Functions from the public interface of basicThermo and
turbulenceModel have been added (like kappa, kappaEff etc)
With the parameter
constructUnconditionally yes;
in function objects that start with executeIf it is possible to
construct the lists unconditionally at start instead of waiting
for the condition to be true. If unset then the function objects
default to the old behaviour
The regular behavior for this function object is that it does
the first manipulation during construction. This can be switched
off with the setting manipulateAtStartup in cases where not all
the requirements for correctly evaluating the expressions are
fulfilled during construction
The utility can now read surface and point fields. Surface-fields are not corrected because this is not supported by Foam
The utility now reads fvOptions for FOAM-versions that support
it. They have to be switched on with ‘useFvOptions’ as most of
the tine they are not needed (only with function objects that
solve equations)
When this option is set then the function-objects are read (including the field) but never solved
The utility now reports the time. This is useful when using the utility to test function objects
The function objects solveLaplacianPDE and solveTransportPDE
now have a new parameter sourceImplicitUseSuSp that allows
switching from using Sp() (the default) to SuSp() for the
addition of sourceImplicitExpression
The command line option -useDynamicMesh tells the utility to
read the mesh as a dynamic mesh and update it at every time-step
If the function object detects that it is created with a moving
mesh then it asks for a parameter makePhiRelative to specify
whether phi should be made relative to the mesh movement (this
is usually necessary). Then either a velocityExpression or a
velocityName has to be specified as well and phi is corrected
according to the mesh movement
If steady is true then phi is not made relative
If a cloud is created and in en entry in expressions the entry
class is found then it is assumed that a field of that type
should be created. The expression is not evaluated but added to
the cloud for each particle.
Note: this does not do any semantic checking and is only to
be used to set constant values for required fields for which
swak can not evaluate the type
For some reason the linear solver does not converge on the
solveTransportPDE and solveLaplacianPDE function
objects. This messes up the solution field. In these cases the
solution field is reset to the last known good solution. If this
behavior is undesired it can be switched off with
restoreNonConvergedSteady
There are now three more options for outputControlMode:
outputTimeAndStartup, timeStepAndStartup and
deltaTAndStartup. These work like the other options but write
data at the startup-time as well
This function object used to only dump values from the master processor if used in parallel. Now the values from all processors are dumped in the order of the processors
Two properties that were missing for that cloud type are now available in the parser
This case has been modified to a version that was presented at
the PFAU (Austrian User Group Meeting) in 2015. Now it compares
with the scalarTransport function object that was added to
OpenFOAM.
The case now also calculates the time the fluid needs from the
inlet to the outlet (residenceTime). Steady as well as
transient
This version is supported in the this version of
swak4Foam. There is only one problem: there were changes to the
tmp-template. These changes have been taken care of in the
swak4Foam-sources. But there are two source files in the
distro that need to be modified (basically adding .ref()
instead of () in three places:
src/finiteVolume/finiteVolume/fvc/fvcD2dt2.C src/finiteVolume/fvMatrices/fvMatrix/fvMatrixSolve.C
Therefor the officially released version will never compile
with swak4Foam but this is nothing that can be fixed in
swak4Foam (the patch is found in the directory
distroPatches/OpenFOAM-v1606+)
This version is supported in this version of swak4Foam. There is
one problem: the released version has two problems that mean that
swak4foam will never compile on the released version.
Patches fixing these issues are found in the directory
distroPatches/OpenFOAM-4.0
This version is supported in this version of swak4Foam. No
modifications are required
This version supports OpenFOAM v1612+. The modifications were done by Mark Olesen
The location of files written by these function objects (which
are almost all function objects writing data in the
postProcessing-directory) has changed: now if the function
object belongs to a region that is not the default mesh the
output is written to a sub-directory with the name of that mesh.
This might break scripts or other tools that people use to process that data
On some distros the destruction of a field stored in an autoPtr
after the destruction of the mesh causes an error message. This
has no effect but is annoying. Fixed
The function object was executed every time not matter what
outputControlMode was set. Fixed
Until now only the internalField and the faInternalField
supported boolean results. Now all drivers support them
Because the static variable/method driverName was not specified
no plugin functions for clouds could get specified
If a primitive function for instance expects a label and finds an
unscanable string like x23 then this used to generate a failure
by the C++-library. This gave no indication on the real
problem. Now there is a OpenFOAM-error message with a somewhat
better explanation
Because of the wrong order of initialization of these function objects they failed in parallel. Fixed
This war reported by Philippose Rajan (who also provided a patch) at https://sourceforge.net/p/openfoam-extend/ticketsswak4foam/237/
In parallel if the values was marked as a single value but no
part of the underlying entity was on the processor it was tried
to access the first element of an empty field. The fix was to
write the value
If the patch version of the current OpenFOAM-version is not a
number and not x then this function object failed
As patch types like empty have no values stored this plugin
failed. Now it checks if there is data
When storing the data for the function object no reference to the parent directory was stored and therefor scoped macro-expansion did not work anymore
The thermophysical functions in this plugin did not work if
thermoType was a dictionary. Fixed
Also: construction of turbulence now gets the rho-field directly from the thermophysics
Reason was that only two specific thermo-subtypes of
fluidThermo were searched if the method was not part of
solidThermo. Now also the basic type is searched
The drivers for sampled entities, sets and zones found global variables but were not able to use them correctly. Fixed
The reason is that when constructing the CloudProxy a cast is
made to the assumed cloud type which in the case of cloud
function-objects is not the actual type. To avoid this separate
instantiations of the CloudProxy were added
To fix a problem with writing of single values in parallel (see
above) a union was added to store the single values. The reason
for this is to avoid a second parallel communication when writing
the value. This adds memory to ExpressionResult (in the order
of a tenor object). The memory is not the problem but that the
single value is saved twice (the other time is in the regular
value field)
For compilers that do not support the C++0x-standard instead of a
union a struct will be used because non-primitive members for
unions are only supported for that standard. This will lead to
a slightly higher memory usage (but still small compared to full
fields)
OpenFOAM-versions based on the foundation release 4.0 and later
don’t have a start()-method in the function objects
anymore. Lot of functionality of swak relied on this method. To
make swak compatible across versions start() is now called in
the constructors of the function-objects (if the OpenFOAM-version
requires it)
If the compiled version is not a released one then the info of
hg branch is added to the version output that utilities like
funkySetFields print
Different OpenFOAM-versions have different formats for the input
files. This means that examples that work for one version will
break with another version (but is still useful to see how things
are done). The file
Documentation/examplesCompatibilityMatrix.org gives an
(incomplete) overview on which versions run which examples (some
examples will never run because a certain feature might be
missing in that Foam-version)
Currently 4 Foam-versions are tested
- OpenFOAM 4.1 (the Foundation release)
- Foam-extend 4.0
- OpenFOAM+ 1612
- OpenFOAM 2.3 (to check compatibility with old versions)
Other versions might or might not work. The first three will be replaced with the latest version of that fork once it becomes available
When adding the library libswakShiftFieldFunctionPlugin.so to
libs in the controlDict functions are added that allow
shifting volume fields by a specified distance. One example
would be an expression
"shiftConstantScalarField(T,(1 1 0))"
which generates a new volScalarField where the value at (0 0
0) is the value of T at the location (1 0 0).
The scheme for naming the functions is
scalar<ShiftType><ValueType>Field with
- ValueType
- one of the base types
Scalar,Vector,Tensor,SymmTensor,SphericalTensor - ShiftType
- how the shift is specified. Possible values are either
- Constant
- A constant vector (like the example here)
- Expression
- An expression that gives a
pointVectorField(for instanceinterpolateToPoint(time()*vector(0,0,-1)))
These functions work by generating a new mesh that is shifted as specified (in the inverse direction) and interpolating between this and the original mesh. This is computationally very expensive and therefor not recommended in evaluations that occur very often.
Cells that have no shifted equivalent value are set to zero. Boundary patches are not interpolated. Both of these behaviors can cause weird results.
There are also variants with Default in the end. These allow
setting different default values than
The functions with the names map<ShiftType><ValueType>Field map
the value of the nearest cell. This is more stable but might
coarsen the field
The additional findShifted<ValueType>Field-functions do the
mapping by avoiding the meshToMesh-functions of OpenFOAM: the
shifted value is found by “looking” into the original cell that
contains the point that is the cell center plus the displacement
value. If that point is not in the mesh a default value is used
This library implements State machines. This is a convenient
way to store a state in a simulation and switch between them by
predefined rules. An example for states in a State machine
would be: closed, valveOpening, open, valveClosing
The library has the function objects and plugin functions to use State machines.
The chapter State machines in the Incomplete swak4Foam reference describes it in more detail
This function object allows modifying fvSchemes and
fvSolution according to the states of two state machines.
All the functions in this plugin first calculate a distribution. This distribution is calculated from the first parameters:
- the field for which the distribution is calculated
- the weight with which the cell values enter the
distribution. Usually
vol()(volume weighted) or1(equal weight for all cells) - a logical expression that specifies which cells are used
(
truefor all cells) - the number of bins to use for the distribution. This specifies
how fine the distribution is calculated. Should be small
compared to the number of cells. Usually the values
100or1000should be sufficient
The implemented functions are
- fracSmallerThan
- Writes a fraction in the range from $0$ to $1$ with for instance $0.5$ meaning “50 % of the distribution is smaller than the value in this cell”. The cells which are masked out get the value $-1$.
- fracSmallerThanFromOther
- Like
fracSmallerThanbut there is an additional parameter: the field that is used for calculating the fraction. Here the mask is not used for calculating the fraction (but still used for calculating the distribution) - quantileFromOther
- Basically the inverse of
fracSmallerThanFromOther. The last parameter is a fraction (from $0$ to $1$) and the result is the corresponding quantile: if a fraction $0.5$ is specified then the value from the distribution for which 50% are smaller is written to the cell
Note: values may slightly vary according to the number of bins. But the bin number also increases the calculation time.
A function outputTime() has been added to the parsers. This
function is true if Foam is writing at the current time and
false else
Sometimes to debug problems with boundary conditions it is good
to look at fields like refValue in Paraview (for instance
because groovyBC might not have set that value the way we
expected it). For a field foo the utility would write a field
foo_bar if the user specified bar to be written. The interior
of the field will be bar is defined will be
fixedValue with the value of bar. All others are
zeroGradient
A string with the specificion of the subfields to create fields
for is set with the option -subfields. The specifications are
separated by ,. Each specification is of the form
<name>:<type> (with type being scalar, vector, symmTensor
or sphericalTensor. A type native assumes that the same type
as the field should be used). If unset the default value is used:
the specification to write all subfields usually associated with
the mixed boundary condition
It is assumed that the length of the sub-field is equal to the number of faces in the patch
This libraries collects specializations of dynamic mesh classes that work together with OpenFOAM. Currently these classes are in the library:
- swakMotion
- this is a solid body motion solver for the
solidBodyMotionFvMeshwhere the translation and the rotation of the solid body can be specified byswak-expressions - groovyCyclicACMI
- this patch type is a subclass of
cyclicACMIwhere the faces that cyclic can be switched on and off with an additional field that is specified with the parameteropenFieldin the specification in theboundary-file. This field has to be present in memory at the first time-step (usually areadAndUpdateFields-functionObject is a good way to achieve this). The values on the correspondingnonOverlapPatchof the first boundary in the coupled pair is used to switch faces on and off: if the value of the face is $1$ then it is ‘open’ if it is $0$ it is ‘closed’ - nonMovingFvMesh
- A non-moving mesh that pretends to move. This triggers the recalculation of AMI-interfaces
- groovyBCJumpAMI
- allows implementing a jump condition on an AMI-interface that depends on an expression evaluated on the master patch of the interface
The folder Examples/DynamicMesh has examples for this library
The two fvOptions matrixChangeBefore and matrixChangeAfter
can be used to record the residual or the change of it.
The residual
matrixChangeBefore calculates this for a fieldName and uses for fvMatrix of
that field. The result is stored in a field whose name is
composed of the value of namePrefix and fieldName. This field
can be useful to see where the current solution does not fit the
linearized system
matrixChangeAfter does the same calculation but assumes that
the field already exists and subtracts the result from the
previous value. So if another fvOption was applied to the
fvMatrix between these calls then the field has the change of
this matrix. If “only” a source term was added then this field
corresponds to the source term.
In principle fvOptions are executed in the order in which they
are specified. If the setting doAtAddSup is set to true then
it is executed in an early phase (when source terms are set). If
set to false then the fvOption is executed during the
setValues=/=constrain phase.
This new function object in simpleSwakFunctionObjects evaluates
a scalar expression and sets deltaT accordingly. Only works
on OpenFOAM-versions that support DataEntry or its successor
Function1Types.
The parser for primitve types now supports tensor,
symmTensor and sphericalTensor as well.
For an expression fooFunmction(var+2) where fooFunction is a
Plugin-function the symbol var can now be a variable: if in the
parent dictionary there is a sub-dictionary fooFunctionData
then this dictionary is searched for a variables-entry and
these variables are then evaluated (it is also possible to have
lookuptables and similar in fooFunctionData)
Function objects that inherit from timelineFunctionObject (like
swakExpression) now have an optional parameter
writeStartTime. If set to yes then the value at start-time
will be written. The default setting is no. This is similar to
the old behavior and avoids crashes at startup. Some classes
change this default to make it yes
Additional functions for the absorptionEmissionModel and the
sootModel are added to to library with the radiation-functions
The function object readAndUpdateFields got three improvements:
- an optional switch
correctBoundaryallows switching the correction of boundary conditions off - surface-fields are now read as well. But no boundary correction is performed as the these fields do not support this
- better output. Instead of silently reading fields or using those in memory the name of the field and the type are written out
Normally the function object only executes only if this is the
real start time (not a restart). If the option executeOnRestart
is set then the function object also executes if this is a restart
On OpenFOAM-versions that support it this now reports if
constrain is called for an equation
In earlier OpenFOAM-versions the name of this method was
setValue. To keep source compatibility this method is kept and
the method constrain patches through to it. If the fvOption
has SetValue in the name then this name is kept
To conform with the way that regular OpenFOAM function objects do
it now function objects that belong to the non-default mesh in
multi-region cases write their data to a sub-directory of
postProcessing named after the mesh
Function objects can now be loaded with an option
-allowFunctionObjects
Normally the function object only executes only if this is the
real start time (not a restart). If the option executeOnRestart
is set then the function object also executes if this is a restart
When reading these data structures the parent directory is
correctly passed and therefor scoped macro expansions
($[:deltaT] for instance) works
Demonstrates getting changes to the solution (residuals) with
matrixChangeBefore and matrixChangeAfter
- Examples/StateMachine/stateCavity
- demonstrates the basic functionality of state machines
- Examples/manipulateFvSolutionFvSchemes/pitzDailyStateMachineSwitched
- demonstrates using state machines to manipulate the discretization during a simulation
The folder Examples/DynamicMesh has examples that demonstrate
capabilities of the swakDynamicMesh-library.
- rotatingTank2D
- is a demonstration of a
solidBodymesh movement where translation and rotation are described by swak-expressions - hecticInletACMI2D,switchedTJunction,switchedInletACMI2D
- demonstrate
a
ACMIboundary condition where switching of faces is done by a swak-expression. Won’t work withFoam-extendas this has noACMI
Minor adaptions were required to make this compile
Some adaptions were required to make this compile
Minor adaptions were required to make this compile by Mark Olesen
The field name is now the name of the original field plus
Potential. This means that in fvSchemes discretizations for
that field have to be provided
Here the function object failed with a “copy to myself”-error. This has been fixed by changing the name of the temporary field.
When finding a cutting point in “infinity” then magSqr
failed. Fixed
The atan2(x,y) function has been added to all the parsers. This
takes 2 values of which one must be non-zero (they represent a
point in the