OpenFOAM offers the capability for post-processing OpenFOAM cases with Fieldview. The
method involves running a post-processing utility foamToFieldview to convert case
data from OpenFOAM to Fieldview .uns file format. For a given case, foamToFieldview is
executed like any normal application, either from FoamX, or from a terminal
window by a command of the form:
foamToFieldview<root><case>
foamToFieldview creates a directory named Fieldview in the case directory,
deleting any existing Fieldview directory in the process. By default the
converter reads the data in all time directories and writes into a set of files of
the form <case>_nn.uns, where nn is an incremental counter starting
from 1 for the first time directory, 2 for the second and so on. The user
may specify the conversion of a single time directory with the option
-time <time>, where <time> is a time in general, scientific or fixed
format.
Fieldview provides certain functions that require information about
boundary conditions, e.g. drawing streamlines that uses information about
wall boundaries. The converter tries, wherever possible, to include this
information in the converted files by default. The user can disable the
inclusion of this information by using the -noWall option in the execution
command.
The data files for Fieldview have the .uns extension as mentioned already. If the
original OpenFOAM case includes a dot ‘.’, Fieldview may have problems interpreting a
set of data files as a single case with multiple time steps.
