G98 -Feed Per Minute(Feed/M) , G99 -Feed Per Rev(Feed/R) - GSK GSK928TEa User Manual

Programming
The above two examples are programmed according to the actual shape, Fig. 4-42a: its
programming can be used to the roughing including smithing and moulding, which can improve the
machining efficiency. Fig. 4-42b: it can be used to machining the rod
4.17 G98 —Feed per Minute(feed/m) , G99 —Feed per Rev(feed/r)
【Command format】
G98 F＊＊＊＊＊. ＊＊＊ ; feed per minute
G99 F＊＊＊＊＊. ＊＊＊ ; feed per rev
【Field】
G98 F＊＊＊＊＊. ＊＊＊ ; F unit：mm/min;
F －define the feedrate of its following interpolation command, its unit: mm/min.
G99 F＊＊＊＊＊. ＊＊＊ ; F unit：mm/r;
F － define the feedrate of its following interpolation command, its unit: mm/r.
【Field range】
F：0～15000.000mm/min
0～15000.000mm/r
【Note】
G98/G99 must be matched with F word， otherwise the system alarms： "F leaves out information".
1)
G98/G99 is the modal command and it is valid before being changed. The single F can be taken
2)
as the new feedrate.
G98 is the initial state of system and the system automatically sets as G98 (mm/min).
3)
F=0: the system alarms and prompts the alarm message when it executes the machining
4)
programs.
In G99, when the spindle speed is 0, the feed automatically pauses and the system displays
5)
"Pause: the spindle speed is 0", keeps the state till the spindle speed is not zero, then, press
CYCLE START again, the system recovers the execution.
In G99, generally, when the spindle is started just now, the system should delay time properly to
6)
wait the spindle speed stably and executes the cutting, otherwise, the system has not checked
the spindle speed, displays "Pause: the spindle speed is 0".
【Example】
...
N0100 G98 F800
...
N0160 F50
...
N0200 G99 F2.1
...
N0250 F0.56
...
Chapter Four
; define the feed per minute，F feedrate: 800 mm/min;
; F feedrate: 50 mm/min;
; set the feed per rev，F feedrate: 2.1 mm/rev;
; F feedrate: 0.56 mm/rev.
G Commands and Functions
235