Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 453)

Programming Feedrates
Chapter 18
18-5
In the G94 mode (feed--per--minute), the numeric value following address
F represents the distance the axis or axes move (in inches or millimeters)
per minute. If the axis is a rotary axis, the F--word value represents the
number of degrees the axis rotates per minute.
To request a feedrate of 35.5 mm of tool motion per minute, program:
G94 G21 F35.5;
Figure 18.4
Feed Per Minute Mode (G94)
Cutting
tool
F
rate/min
Workpiece
Table
When changing from G93 or G95 modes to G94 mode, an feedrate must be
programmed in the initial G94 block.
Since the G94 code is modal, it remains active until canceled by the G93 or
G95 mode. Any F--word programmed while G94 mode is active will be
considered a feed per minute feedrate.
In G95 (feed--per--revolution) mode, the numeric value following the F--
address represents the distance the axis or axes move (in inches or
millimeters) per spindle revolution. If the axis is a rotary axis, the F--word
value represents the number of degrees the axis rotates per spindle
revolution.
To request a feedrate of 1.5 mm per spindle revolution, program:
G95 G21 F1.5
18.1.3
Feed- Per- Minute Mode
(G94)
18.1.4
Feed- Per- Revolution Mode
(G95)