Introduction🔗
OpenFOAM solver applications typically include core functionality such as turbulence modelling, heat transfer, and buoyancy effects.
Further flexibility is offered via fvOptions
—a collection of run-time
selectable finite volume options to manipulate systems of equations by adding
sources/sinks, imposing constraints and applying corrections.
These are specified in the fvOptions file located in the $FOAM_CASE/system or $FOAM_CASE/constant directories.
Options🔗
Usage🔗
Selecting the region🔗
The majority of options are applied to collections of mesh cells. These can
be selected according to the entry selectionMode
, e.g.
selectionMode all;
Valid selectionMode
entries include:
-
all
: all cells -
cellZone
: cells defined by a cell zone. This requires an additional entry to specify the name of the cell zone, e.g.
selectionMode cellZone;
cellZone myCellZone;
where myCellZone
is the name of the cell zone
-
cellSet
: cells defined by a cell set. This requires an additional entry to specify the name of the cell set, e.g.
selectionMode cellSet;
cellSet myCellSet;
where myCellSet
is the name of the cell set.
-
points
: a list of points. This requires an additional entry to list the points, e.g.
selectionMode points;
points ((0 0 0) (1 1 1) (2 2 2));