-
Henry Weller authored
with the more general and flexible 'postProcess' utility and '-postProcess' solver option Rationale --------- Both the 'postProcess' utility and '-postProcess' solver option use the same extensive set of functionObjects available for data-processing during the run avoiding the substantial code duplication necessary for the 'foamCalc' and 'postCalc' utilities and simplifying maintenance. Additionally consistency is guaranteed between solver data processing and post-processing. The functionObjects have been substantially re-written and generalized to simplify development and encourage contribution. Configuration ------------- An extensive set of simple functionObject configuration files are provided in OpenFOAM-dev/etc/caseDicts/postProcessing and more will be added in the future. These can either be copied into '<case>/system' directory and included into the 'controlDict.functions' sub-dictionary or included directly from 'etc/caseDicts/postProcessing' using the '#includeEtc' directive or the new and more convenient '#includeFunc' directive which searches the '<etc>/caseDicts/postProcessing' directories for the selected functionObject, e.g. functions { #includeFunc Q #includeFunc Lambda2 } '#includeFunc' first searches the '<case>/system' directory in case there is a local configuration. Description of #includeFunc --------------------------- Specify a functionObject dictionary file to include, expects the functionObject name to follow (without quotes). Search for functionObject dictionary file in user/group/shipped directories. The search scheme allows for version-specific and version-independent files using the following hierarchy: - \b user settings: - ~/.OpenFOAM/\<VERSION\>/caseDicts/postProcessing - ~/.OpenFOAM/caseDicts/postProcessing - \b group (site) settings (when $WM_PROJECT_SITE is set): - $WM_PROJECT_SITE/\<VERSION\>/caseDicts/postProcessing - $WM_PROJECT_SITE/caseDicts/postProcessing - \b group (site) settings (when $WM_PROJECT_SITE is not set): - $WM_PROJECT_INST_DIR/site/\<VERSION\>/caseDicts/postProcessing - $WM_PROJECT_INST_DIR/site/caseDicts/postProcessing - \b other (shipped) settings: - $WM_PROJECT_DIR/etc/caseDicts/postProcessing An example of the \c \#includeFunc directive: \verbatim #includeFunc <funcName> \endverbatim postProcess ----------- The 'postProcess' utility and '-postProcess' solver option provide the same set of controls to execute functionObjects after the run either by reading a specified set of fields to process in the case of 'postProcess' or by reading all fields and models required to start the run in the case of '-postProcess' for each selected time: postProcess -help Usage: postProcess [OPTIONS] options: -case <dir> specify alternate case directory, default is the cwd -constant include the 'constant/' dir in the times list -dict <file> read control dictionary from specified location -field <name> specify the name of the field to be processed, e.g. U -fields <list> specify a list of fields to be processed, e.g. '(U T p)' - regular expressions not currently supported -func <name> specify the name of the functionObject to execute, e.g. Q -funcs <list> specify the names of the functionObjects to execute, e.g. '(Q div(U))' -latestTime select the latest time -newTimes select the new times -noFunctionObjects do not execute functionObjects -noZero exclude the '0/' dir from the times list, has precedence over the -withZero option -parallel run in parallel -region <name> specify alternative mesh region -roots <(dir1 .. dirN)> slave root directories for distributed running -time <ranges> comma-separated time ranges - eg, ':10,20,40:70,1000:' -srcDoc display source code in browser -doc display application documentation in browser -help print the usage pimpleFoam -postProcess -help Usage: pimpleFoam [OPTIONS] options: -case <dir> specify alternate case directory, default is the cwd -constant include the 'constant/' dir in the times list -dict <file> read control dictionary from specified location -field <name> specify the name of the field to be processed, e.g. U -fields <list> specify a list of fields to be processed, e.g. '(U T p)' - regular expressions not currently supported -func <name> specify the name of the functionObject to execute, e.g. Q -funcs <list> specify the names of the functionObjects to execute, e.g. '(Q div(U))' -latestTime select the latest time -newTimes select the new times -noFunctionObjects do not execute functionObjects -noZero exclude the '0/' dir from the times list, has precedence over the -withZero option -parallel run in parallel -postProcess Execute functionObjects only -region <name> specify alternative mesh region -roots <(dir1 .. dirN)> slave root directories for distributed running -time <ranges> comma-separated time ranges - eg, ':10,20,40:70,1000:' -srcDoc display source code in browser -doc display application documentation in browser -help print the usage The functionObjects to execute may be specified on the command-line using the '-func' option for a single functionObject or '-funcs' for a list, e.g. postProcess -func Q postProcess -funcs '(div(U) div(phi))' In the case of 'Q' the default field to process is 'U' which is specified in and read from the configuration file but this may be overridden thus: postProcess -func 'Q(Ua)' as is done in the example above to calculate the two forms of the divergence of the velocity field. Additional fields which the functionObjects may depend on can be specified using the '-field' or '-fields' options. The 'postProcess' utility can only be used to execute functionObjects which process fields present in the time directories. However, functionObjects which depend on fields obtained from models, e.g. properties derived from turbulence models can be executed using the '-postProcess' of the appropriate solver, e.g. pisoFoam -postProcess -func PecletNo or sonicFoam -postProcess -func MachNo In this case all required fields will have already been read so the '-field' or '-fields' options are not be needed. Henry G. Weller CFD Direct Ltd.e4dc50dc
Mach 1.52 KiB
#!/bin/sh
#------------------------------------------------------------------------------
# ========= |
# \\ / F ield | OpenFOAM: The Open Source CFD Toolbox
# \\ / O peration |
# \\ / A nd | Copyright (C) 2016 OpenFOAM Foundation
# \\/ M anipulation |
#-------------------------------------------------------------------------------
# License
# This file is part of OpenFOAM.
#
# OpenFOAM 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 3 of the License, or
# (at your option) any later version.
#
# OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
# ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
# FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License
# for more details.
#
# You should have received a copy of the GNU General Public License
# along with OpenFOAM. If not, see <http://www.gnu.org/licenses/>.
#
# Script
# Mach
#
# Description
# Script to suggest using the new "-postProcess" solver option.
#
#------------------------------------------------------------------------------
Script=${0##*/}
echo $Script "has been superceded by the -postProcess solver option:"
echo "<solverName> -func MachNo"
echo "e.g."
echo "sonicFoam -postProcess -func MachNo"
#------------------------------------------------------------------------------