Difference between revisions of "Contrib multiSolver/Post processing"

Revision as of 16:39, 1 July 2011

multiSolver has a post processing tool with the same name, which is required to make data available to the standard post processors.

1 Overview

OpenFOAM is hard-coded to look for data in the case/[time] directories. In order to post-process (including sampling, and data conversion) the data needs to be there. To accomplish this, a post processing utility is available. Typing the command multiSolver in the terminal accesses this. It has four main commands:

• -load - copy data files from their storage location to case/time (i.e. load the data for post-processing);
• -purge - delete data files;
• -list - display the contents found in the case directory storage location; and
• -set - make the case directory appear as required for the given solver name.

2 Syntax

multiSolver -command 'options' [-global] [-local] [-noPurge] [-noSet] [-noStore]

3 -command

Choose one of:

• list - list data available
• load - copy specified data to case/time
• purge - delete specified data
• set - change case directory to match supplied solver domain

3.1 list

Takes no options. Giving options will produce an error.

multiSolver -list

3.2 load

Loads the data specified in options. Additional options:

• -global, -local - By default, load will copy by localTime, unless the times overlap, in which case it loads by globalTime. These options force it to load by the specified time.

• -noPurge - By default, load will purge the case/time directories before copying the new data in. This option disables this behaviour.

• -noSet - By default, if all the specified load data is from a single solverDomain, load will automatically set the case directory to this solverDomain. This option disables this behaviour.

• -noStore - By default, if any storeFields exist, they will be copied into every time directory in which they are missing - this is for ease of post-processing. This option disables this copying, leaving only the data that actually exists in the multiSolver directory.

Load all data:

multiSolver -load all

Load all data from icoFoam solverDomain, using globalTime.

multiSolver -load icoFoam -global

Load all data from scalarTransportFoam, superLoops 1, 2, and 5 through 9, but do not delete the case/time directories first:

multiSolver -load 'scalarTransportFoam 1 2 5:9' -noPurge

3.3 purge

Purges the data specified in options.

Delete all the case/time directories:

multiSolver -purge root

Delete superloops 5 through 9 in all solverDomains:

multiSolver -purge '5:9'

Delete all data in all solverDomains (except for initial directories):

multiSolver -purge all

3.4 set

Sets the case directory to a given solverDomain. That is, all multiDicts are changed to the correct solverDomain; and a controlDict is written. The controlDict doesn't have all the data for the given solverDomain, but it (importantly) points to the first case/time directory as its startFrom. paraFoam uses this to initialize.

Set can only take a single solverDomain in options. Any superLoop specifications, or additional solverDomain names will result in error.

4 'options'

The options to the command. If the options have whitespace characters (i.e. are more than 1 word), they must be enclosed in apostrophes. Options come in two parts: solverDomains, followed by superLoops. Each can have any number of entries, including zero, but options cannot be empty unless using -list.

4.1 solverDomainNames

A simple word list, space delimited. List any solverDomains you want to load data from. e.g.:

scalarTransportFoam icoFoam customSolver

or

icoFoam

Omitting solverDomainNames indicates that *all* solverDomains will be used.

4.2 superLoop numbers

A space delimited number list in any order. Can include ranges using a : character. A value of -1 indicates the initial directory. e.g.:

3 5 6 9:12

or

-1 5

Omitting superLoop numbers entirely indicates that *all* superLoops will be used.

4.3 Special words

There are two special words reserved for some of the commands:

• all - indicates all solverDomains and all superLoops. Useable by -load and -purge.
• root - indicates all case/time directories. Useable by -purge only.

e.g.:

multiSolver -load all
multiSolver -purge root

5 Examples

Show all available data:

multiSolver -list

Load all available data:

multiSolver -load all

Load all data from solverDomain icoFoam:

multiSolver -load icoFoam

Load all data from superLoops 8 and 9 from all solverDomains:

multiSolver -load '8 9'

Load all data from superLoops 4, 6, 7, 8, and 9 from solverDomain scalarTransportFoam, but do not delete any existing case/time directories.

multiSolver -load 'scalarTransportFoam 4 6:9' -noPurge

Load all data from superLoops 4, 5, 7, 8 and 9 from solverDomains icoFoam and scalarTransportFoam, but force the directory names to globalTime:

multiSolver -load 'icoFoam scalarTransportFoam 4 5 7:9' -global

Delete all case/time directories:

multiSolver -purge root

Delete all time directories in case/multiSolver/allSolverDomains/allSuperLoops, but do not delete any initial directories:

multiSolver -purge all

Delete superLoops 5, 6, 7, 8, and 9 from all solverDomains:

multiSolver -purge '5:9'

This instruction says to delete the initial directory from solverDomain icoFoam, but the initial directory is never deleted, therefore nothing is done:

multiSolver -purge 'icoFoam -1'

Set the case directory to scalarTransportFoam's settings:

multiSolver -set scalarTransportFoam