Siemens SINUMERIK 840D sl Programming Manual page 139

NOTICE
Tool operations undefined
Technological concerns such as climb milling or conventional milling, front face milling or
peripheral face milling, etc., along with the path geometry (straight line, circle, etc.), are not
taken into account automatically. Therefore, these factors have to be given consideration
when programming the tooth feedrate.
Note
Switchover between G95 F... and G95 FZ...
With switchover between G95 F... (revolution feedrate) and G95 FZ... (tooth feedrate), the
inactive feedrate value is deleted in each case.
Note
Derive feedrate with FPR
As is the case with the revolutional feedrate, FPR can also be used to derive the tooth feedrate
of any rotary axis or spindle (see "Feedrate for positioning axes / spindles (FA, FPR, FPRAON,
FPRAOF) (Page 122)").
Examples
Example 1: 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
...
Example 2: Switchover between G95 F... and G95 FZ...
Program code
N10 G0 X100 Y50
N20 G1 G95 F0.1
N30 T1 M6
N35 M3 S100 D1
N40 X20
N50 G0 X100 M5
NC programming
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
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
Comment
; Revolutional feedrate 0.1 mm/rev
Fundamentals
2.7 Feed control
139