Siemens SINUMERIK 840D Function Manual page 129

Revolutional feedrate (G95)
The revolutional feedrate is programmed in the following units relative to a master spindle:
● [mm/rev] on standard metric systems
● [inch/rev] on standard imperial systems
● [degrees/rev] on a rotary axis
The path velocity is calculated from the actual speed of the spindle according to the following
formula:
V = n * F
with
Note
The programmed F value is deleted when the system switches between the feedrate types
G93, G94 and G95.
Tooth feedrate
Primarily for milling operations, the tooth feedrate FZ... (feed distance per tooth), which is
more commonly used in practice, can be programmed instead of the revolutional feedrate
F...:
The control system uses the $TC_DPNT (number of teeth per revolution) 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 * $TC_DPNT
with
Example: Milling cutter with 5 teeth ($TC_DPNT = 5)
Program code
N10 G0 X100 Y50
N20 G1 G95 FZ=0.02
N30 T3 D1
M40 M3 S200
N50 X20
Axes and spindles
Function Manual, 06/2019, A5E47437747B AA
Path velocity in mm/min or inch/min
V:
Speed of the master spindle in rpm
n:
Programmed revolutional feedrate in mm/rev or inch/rev
F:
Revolutional feedrate in mm/rev or inch/rev
F:
Tooth feedrate in mm/tooth or inch/tooth
FZ:
Tool parameter: Number of teeth/rev
$TC_DP
NT:
Comment
; Tooth feedrate 0.02 mm/tooth
; Load tool and activate tool offset data block.
; Spindle speed 200 rpm
; Milling with FZ = 0.02 mm/tooth
; effective revolutional feedrate:
; F = 0.02 mm/tooth * 5 teeth/rev = 0.1 mm/rev
; or:
; F = 0.1 mm/rev * 200 rpm = 20 mm/min
V1: Feedrates
5.2 Path feedrate F
129