OpenFOAM v9 User Guide - 4.7 Case management tools

4.7 Case management tools

There are a set of applications and scripts that help with managing case files and help the user find and set keyword data entries in case files. The tools are described in the following sections.

4.7.1 File management scripts

The following tools help manage case files.

foamListTimes

lists the time directories for a case, omitting the 0 directory by default; the -rm option deletes the listed time directories, so that a case can be cleaned of time directories with results by the following command.

    foamListTimes -rm

foamCloneCase

creates a new case, by copying the 0, system and constant directories from an existing case; executed simply by the following command, where oldCase refers to an existing case directory.

    foamCloneCase oldCase newCase

4.7.2 foamDictionary and foamSearch

The foamDictionary utility offer several options for writing, editing and adding keyword entries in case files. The utility is executed with an OpenFOAM case dictionary file as an argument, e.g. from within a case directory on the fvSchemes file.

Without options, the utility lists all the keyword entries in the file, e.g. as follows for the fvSchemes file in the pitzDaily tutorial case for simpleFoam.

The -entry option allows the user to print the entry for a particular keyword, e.g. divSchemes in the example below

The example clearly extracts the divSchemes dictionary.

The “/” syntax allows access to keywords with levels of sub-dictionary. For example, the div(phi,U) keyword can be accessed within the divSchemes sub-dictionary by the following command.

The example returns the single divSchemes/div(phi,U) entry.

The -value option causes only the entry to be written.

The example removes the keyword and terminating semicolon, leaving just the data.

The -keywords option causes only the keywords to be written.

The example produces a list of keywords inside the divSchemes dictionary.

The example removes the keyword and terminating semicolon, leaving just the data.

foamDictionary can set entries with the -set option. If the user wishes to change the div(phi,U) to the upwind scheme, they can enter the following.

An alternative “=” syntax can be used with the -set option which is particularly useful when modifying multiple entries:

foamDictionary can add entries with the -add option. If the user wishes to add an entry named turbulence to divSchemes with the upwind scheme, they can enter the following.

The foamSearch script, demonstrated extensively in section 4.5 , uses foamDictionary functionality to extract and sort keyword entries from all files of a specified name in a specified dictionary. The -c option counts the number of entries of each type, e.g. the user could searche for the choice of solver for the p equation in all the fvSolution files in the tutorials.

The search shows GAMG to be the most common choice in all the tutorials.

4.7.3 The foamGet script

The foamGet script copies configuration files into a case quickly and conveniently. The user must be inside a case directory to run the script or identify the case directory with the -case option. Its operation can be described using an example case, e.g. the pitzDaily case which can be obtained as follows:

The mesh is generated for the case by going into the case directory and running blockMesh: The user might decide before running the simulation to configure some automatic post-processing as described in Section 6.2 . For example, the user can list the pre-configured function objects by the following command: From the output, the user could select the patchFlowRate function to monitor the flow rate at the outlet patch. The patchFlowRate configuration file can be copied into the system directory using foamGet: In order to monitor the flow through the outlet patch, the patch entry in patchFlowRate file should be set as follows: The patchFlowRate configuration is then included in the case by adding to the functions sub-dictionary in the controlDict file:

4.7.4 The foamInfo script

The foamInfo script provides quick information and examples relating to a subject that the user specifies. The subject can relate to models (including boundary conditions and packaged function objects), applications and scripts. For example, it prints information about the simpleFoam solver by typing the following:

Information for the flowRateInletVelocity boundary condition can similarly be obtained by typing the following: The output includes: the location of the source code header file for this boundary condition; the description and usage details from the header file; and, a list of example cases that use the boundary condition.

The example usage for volumetric flow rate can be copied to replace the inlet boundary condition in the pitzDaily example from Section 4.7.3 . The volumetric flow rate, equivalent to a uniform flow speed of 10 m/s, is so the modified inlet patch entry in the U file in the 0 directory should be:

The simpleFoam solver can then be run. The solution at convergence (around 280 steps), visualised in ParaView, shows a nonuniform velocity profile at the inlet, due to the extrapolateProfile being switched on. The flow rate at the outlet, from the function object set up in Section 4.7.3 , is written to a surfaceFieldValue.dat file in the postProcessing/patchFlowRate/0 directory. The value converges towards the inlet flow rate.