Siemens SINUMERIK 828D Programming Manual page 155

Examples
Example 1: Milling cutter with 5 teeth ($TC_DPNE = 5)
Program code
N10 G0 X100 Y50
N20 G1 G95 FZ=0.02
N30 T3 D1
M40 M3 S200
N50 X20
...
Example 2: Switchover between G95 F... and G95 FZ...
Program code
N10 G0 X100 Y50
N20 G1 G95 F0.1
N30 T1 M6
N35 M3 S100 D1
N40 X20
N50 G0 X100 M5
N60 M6 T3 D1
N70 X22 M3 S300
N80 G1 X3 G95 FZ=0.02
...
Example 3: Derive tooth feedrate of a spindle (FBR)
Program code
...
N41 FPR(S4)
N51 G95 X51 FZ=0.5
...
Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
Comment
; Tooth feedrate 0.02 mm/tooth
; Load tool and activate tool offset data record.
; Spindle speed 200 rpm
; Milling with:
FZ = 0.02 mm/tooth
⇒ effective revolutional feedrate:
F = 0.02 mm/tooth * 5 teeth/rev = 0.1 mm/rev
or:
F = 0.1 mm/rev * 200 rpm = 20 mm/min
Comment
; Revolutional feedrate 0.1 mm/rev
; Load tool with e.g. 5 teeth ($TC_DPNT = 5).
; Change G95 F... to G95 FZ..., tooth feedrate active with
0.02 mm/tooth.
Comment
; Tool in spindle 4 (not the master spindle).
; Tooth feedrate 0.5 mm/tooth dependent upon spindle S4.
Feed control
7.12 Tooth feedrate (G95 FZ)
155