Programming principles
1.3 Axis movements
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0
55
1.3.16 Dwell Time: G4
Functionality
Between two NC blocks you can interrupt the machining process for a defined period by
inserting your own block with G4; e.g. for relief cutting.
Words with F... or S... are only used for times in this block. Any previously programmed
feedrate F or a spindle speed S remain valid.
Programming
G4 F... ; Dwell time in seconds
G4 S... ; Dwell time in spindle revolutions
Programming example
N5 G1 F3.8 Z-50 S300 M3 ;Feed F; spindle speed S
N10 G4 F2.5 ; Dwell time 2.5 seconds
N20 Z70
N30 G4 S30 ;dwelling 30 revolutions of the spindle, corresponds at
; S=300 rpm and 100 % speed override to: t=0.1 min
N40 X20 ;Feed and spindle speed remain effective
N50 M30
Remark
G4 S.. is only possible if a controlled spindle is available (if the speed specifications are also
programmed via S...).
To Next Page
Loading...
Need help?
General
