Tooth Feedrate (G95 Fz) - Siemens SINUMERIK 828D Programming Manual

7.12

Tooth feedrate (G95 FZ)

Function
Primarily for milling operations, the tooth feedrate, which is more commonly used in practice,
can be programmed instead of the revolutional feedrate:
The control uses the $TC_DPNT (number of teeth) tool parameter associated with the
active tool offset data record to calculate the effective revolutional feedrate for each
traversing block from the programmed tooth feedrate.
F = FZ * $TC_DPNT
where:
The tool type ($TC_DP1) of the active tool is not taken into account.
The programmed tooth feedrate is independent of the tool change and the
selection/deselection of a tool offset data record; it is retained in modal format.
A change to the $TC_DPNT tool parameter associated with the active tool cutting edge will
be applied the next time a tool offset is selected or the next time the active offset data is
updated.
Changing the tool or selecting/deselecting a tool offset data set generates a recalculation of
the effective revolutional feedrate.
Note
The tooth feedrate refers only to the path (axis-specific programming is not possible).
Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
F: Revolutional feedrate in mm/rev or inch/rev
FZ: Tooth feedrate in mm/tooth or inch/tooth
$TC_DPNT: Tool parameter: Number of teeth/rev
Feed control
7.12 Tooth feedrate (G95 FZ)
153