Siemens SINUMERIK 840DE Programming Manual page 254

Feedrate Control and Spindle Motion
7.1 Feedrate (G93, G94, G95 or F..., FGROUP, FGREF)
N10 G17 G94 G1 Z0 F500
N20 X10 Y20
N25 FGROUP(X, Y)
N30 G2 X10 Y20 Z-15 I15 J0 F1000
FL[Z]=200
...
N100 FL[Z]=$MA_AX_VELO_LIMIT[0,Z]
N110 M30
Feedrate G93, G94, G95
All of the commands are modal. If the G feedrate command is switched between G93, G94
or G95 the path feedrate must be reprogrammed. The feedrate can also be specified in
deg/rev when machining with rotary axes.
Feedrate F for path axes
The feedrate is specified with address F. Depending on the default setting in the machine
data, the units of measurement specified with the G commands are either in mm or inch.
One F value can be programmed per NC block. The unit for the feedrate is defined in one of
the above G commands. The feed F acts only on path axes and remains active until a new
feedrate is programmed. Separators are permitted after address F.
Example: F100 or F 100 or F.5 or F=2*FEED
7-4
;Tool infeed
;Approach start position
;Axes X/Y are path axes, Z is a
;synchronized axis
;On the circular path, the feedrate is 1000
mm/min.
;Traversing in the Z direction is synchronized.
;The limit velocity is deselected
;when the velocity
;value is read from the MD.
;End of program
Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1
Fundamentals