The basic directory structure for a OpenFOAM case, that contains the
minimum set of files required to run an application, is shown in 4.1 and described
as follows:
Figure 4.1:
Case directory structure
A constantdirectory
that contains a full description of the case mesh in a
subdirectory polyMesh and files specifying physical properties for the
application concerned, e.g.transportProperties.
A systemdirectory
for setting parameters associated with the solution
procedure itself. It contains at least the following 3 files: controlDict
where run control parameters are set including start/end time, time
step and parameters for data output; fvSchemes where discretisation
schemes used in the solution may be selected at run-time; and,
fvSolution where the equation solvers, tolerances and other algorithm
controls are set for the run.
The ‘time’ directories
containing individual files of data for particular
fields. The data can be: either, initial values and boundary conditions
that the user must specify to define the problem; or, results written
to file by OpenFOAM. Note that the OpenFOAM fields must always
be initialised, even when the solution does not strictly require it, as
in steady-state problems. The name of each time directory is based
on the simulated time at which the data is written and is described
fully in 4.3. It is sufficient to say now that since we usually start our
simulations at time , the initial conditions are usually stored in
a directory named 0 or 0.000000e+00, depending on the name format
specified. For example, in the cavity tutorial, the velocity field and
pressure field are initialised from files 0/U and 0/p respectively.
, the initial conditions are usually stored in
a directory named 
and
pressure field 
are initialised from files