Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 449)

Chapter
18
18-1
Programming Feedrates
This chapter describes how to program feedrates and
acceleration/deceleration. Use this table to find the information in this
chapter:
Information about: On page:
Feedrates 18-1
Special AMP Assigned Feedrates 18-12
Automatic Acceleration/Deceleration 18-14
Feedrates are programmed by an F--word followed by a numeric value.
Feedrates can be entered in a part program block or through MDI. They
become effective in the block in which they are programmed. If the block
requires rapid traverse motion (G00), the programmed feedrate will be
ignored for that block, but will be stored in control memory as the active
feedrate.
Feedrates are modal, meaning that they remain active in control memory
unless replaced with a different feedrate programmed with an F--word.
The feedrate programmed with the F--word applies to linear interpolation
(G01), and circular interpolation (G02/G03) modes. For simplification this
manual refers to the cutting tool moving relative to the part, even though
most mills move the part across a stationary cutter.
Feedrate modes are either G93 (inverse time feed), G94 (feed per minute),
or G95 (feed per spindle revolution). The following table shows the
possible feedrate units depending on axis type.
Active G Code Linear Axis Feed Rotary Axis Feed
G20/G21 and G93 moves/min. moves/min.
G02/G03 and G93 radians/min. moves/min.
G21 and G94 millimeters/min. degrees/min.
G20 and G94 inches/min. degrees/min.
G21 and G95 millimeters/rev. degrees/rev
G20 and G95 inches/rev. degrees/rev.
18.0
Chapter Overview
18.1
Feedrates