3.1 Running applications

[prev] [next]

Each application is designed to be executed from a terminal command line, typically reading and writing a set of data files associated with a particular case. The data files for a case are stored in a directory named after the case as described in section 2.1; the directory name with full path is here given the generic name <caseDir>.

For any application, the form of the command line entry for any can be found by simply entering the application name at the command line with the -help option, e.g. typing


    blockMesh -help
returns the usage


Usage: blockMesh [OPTIONS]
options:
  -blockTopology    write block edges and centres as .obj files
  -case <dir>       specify alternate case directory, default is the cwd
  -dict <file>      specify alternative dictionary for the blockMesh description
  -fileHandler <handler>
                    override the file handler type
  -noClean          keep the existing files in the polyMesh
  -noFunctionObjects
                    do not execute function objects
  -region <name>    specify alternative mesh region
  -sets             write cellZones as cellSets too (for processing purposes)
  -doc              display application documentation in browser
  -doc-source       display source code in browser
  -help             print usage information and exit
  -help-full        print full usage information and exit

Block description

  For a given block, the correspondence between the ordering of
  vertex labels and face labels is shown below.
  For vertex numbering in the sequence 0 to 7 (block, centre):
    faces 0 (f0) and 1 are left and right, respectively;
    faces 2 and 3 are bottom and top;
    and faces 4 and 5 are front the back:

           7 ---- 6
      f5   |\     |\   f3
      |    | 4 ---- 5   \
      |    3 |--- 2 |    \
      |     \|     \|    f2
      f4     0 ---- 1

 Z         f0 ----- f1
 |  Y
 | /
 O --- X


Using: OpenFOAM-v1806 (see www.OpenFOAM.com)
Build: v1806
Arch:  "LSB;label=32;scalar=64"
The arguments in square brackets, [ ], are optional flags. If the application is executed from within a case directory, it will operate on that case. Alternatively, the -case <caseDir> option allows the case to be specified directly so that the application can be executed from anywhere in the filing system.

The -help-full offers additional application options. For example the simpleFoam solver offers following extra options:


  -listFunctionObjects
                    List functionObjects
  -listFvOptions    List fvOptions
  -listRegisteredSwitches
                    List switches registered for run-time modification
  -listScalarBCs    List scalar field boundary conditions (fvPatchField<scalar>)
  -listSwitches     List switches declared in libraries but not set in
                    etc/controlDict
  -listTurbulenceModels
                    List turbulenceModels
  -listUnsetSwitches
                    List switches declared in libraries but not set in
                    etc/controlDict
  -listVectorBCs    List vector field boundary conditions (fvPatchField<vector>)

3.1.1 Command line options

Starting from OpenFOAM v1706 the set of command line options can be readily obtained by command-line completion. For example, by pressing the <TAB> key after typing e.g.blockMesh will prompt the list of options.


blockMesh <TAB> <TAB>
Returns:


blockMesh -
-blockTopology      -dict               -help               -noFunctionObjects  -sets
-case               -doc                -noClean            -region             -srcDoc
This functionality is available for for all solvers and utilities.

3.1.2 Running in the background

Like any UNIX/Linux executable, applications can be run as a background process, i.e. one which does not have to be completed before the user can give the shell additional commands. If the user wished to run the blockMesh example as a background process and output the case progress to a log file, they could enter:


    blockMesh > log &

[prev] [next]