Siemens SINUMERIK 840D sl Programming Manual page 138

Fundamentals
2.7 Feed control
The control uses the $TC_DPNT (number of teeth) tool parameter associated with the active
tool offset data block to calculate the effective revolutional feedrate for each traversing block
from the programmed tooth feedrate.
F = FZ * $TC_DPNT
with:
The tool type ($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 block; 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 block generates a recalculation of
the effective revolutional feedrate.
Note
The tooth feedrate refers only to the path (axis-specific programming is not possible).
Syntax
G95 FZ...
Meaning
G95:
FZ:
NOTICE
Tool change/Changing the master spindle
A subsequent tool change or changing the master spindle must be taken into account by the
user by means of corresponding programming, e.g. reprogramming FZ.
138
F: Revolutional feedrate in mm/rev or inch/rev
FZ: Tooth feedrate in mm/tooth or inch/tooth
$TC_DPNT: System variable tool parameter: Number of teeth/rev
Type of feedrate: Revolutional feedrate in mm/rev or inch/rev (dependent upon G700/G710)
For G95 see "Feedrate (G93, G94, G95, F, FGROUP, FL, FGREF) (Page 105)"
Tooth feedrate
Activation: with G95
Effectiveness: Modal
Unit: mm/tooth or inch/tooth (dependent upon G700/G710)
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
NC programming