Siemens SINUMERIK 828D Programming Manual page 156

Feed control
7.12 Tooth feedrate (G95 FZ)
Example 4: Subsequent tool change
Program code
N10 G0 X50 Y5
N20 G1 G95 FZ=0.03
N30 M6 T11 D1
N30 M3 S100
N40 X30
N50 G0 X100 M5
N60 M6 T33 D1
N70 X22 M3 S300
N80 G1 X3
...
Example 5: Changing the master spindle
Program code
N10 SETMS (1)
N20 T3 D3 M6
N30 S400 M3
N40 G95 G1 FZ0.03
N50 X50
N60 G0 X60
...
N100 SETMS(2)
N110 T1 D1 M6
N120 S500 M3
N130 G95 G1 FZ0.03 X20
Note
Following the change in master spindle (
the tool actuated by spindle 2.
156
Comment
; Tooth feedrate 0.03 mm/tooth
; Load tool with e.g. 7 teeth ($TC_DPNT = 7).
; Effective revolutional feedrate 0.21 mm/rev
; Load tool with e.g. 5 teeth ($TC_DPNT = 5).
; Tooth feedrate modal 0.03 mm/tooth
⇒ effective revolutional feedrate: 0.15 mm/rev
Comment
; Spindle 1 is the master spindle.
; Tool 3 is changed to spindle 1.
; Speed S400 of spindle 1 (and, therefore, T3).
; Tooth feedrate 0.03 mm/tooth
; Path motion, the effective feedrate is dependent
upon:
- The tooth feedrate FZ
- The speed of spindle 1
- The number of teeth of the active tool T3
; Spindle 2 becomes the master spindle.
; Tool 1 is changed to spindle 2.
; Speed S500 of spindle 2 (and, therefore, T1).
; Path motion, the effective feedrate is dependent
upon:
- The tooth feedrate FZ
- The speed of spindle 2
- The number of teeth of the active tool T1
) the user also has to select an offset affecting
N100
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
Fundamentals