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: F: Revolutional feedrate in mm/rev or inch/rev
FZ: Tooth feedrate in mm/tooth or inch/tooth
$TC_DPNT: System variable tool parameter: Number of teeth/rev
The tool type ($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: 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)"
FZ: Tooth feedrate
Activation: with G95
Effectiveness: Modal
Unit: mm/tooth or inch/tooth (dependent upon G700/G710)
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.
Fundamentals
2.7 Feed control
NC programming
138 Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
To Next Page
Loading...
Need help?
General
