Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 522)

Cutter Diameter Compensation
(G40, G41, G42)
Chapter 21
21-4
Program the cutter compensation function with the following format:
G41(or G42)X ___ Y ___ Z ___ D ___ ;
Where : Is :
G41(or G42) cutter compensation direction, G41=left, G42=right
X, Y, Z End-point of entry move into cutter compensation. Program an entry
move on axes only in the currently active plane. Axis motion must
take place in order for cutter compensation to be active on an axis.
D Designates the offset numbers and pulls data: 1) from the wear and
geometry tables for the tool radius, and 2) from the geometry table for
tool orientation (see section 20.2.1 for information on programming a
D word). The D word is optional in the G41 or G42 blocks. The D
word may also be designated in any previous or following program
block.
Cutter compensation can be programmed in various ways. Following are
examples of 1-, 2-, and 3-block programs activating cutter compensation
with entry moves.
Example 21.1
Initializing Cutter Compensation
Assume: G17 (XY Plane Selection)
Program Block Comment
One Block
G42 D1 X1 Y1; Sets compensation right, selects tool
radius offset number, and activates move to
X1 Y1
Two Blocks
D1; Selects tool radius offset number
G42 X1 Y1; Sets compensation right and activates move
to X1 Y1
Three Blocks
D1; Selects tool radius offset number
G42; Sets compensation right
X1 Y1; Activates move to X1 Y1
Important: Any entry move (see section 21.3.1 or 21.4.1) into cutter
compensation must be a linear move. Initial activation of cutter
compensation by programming of either the G41 or G42 commands in a
circular cutting mode (G02 or G03) is not allowed. However, if cutter
compensation is already active, the G41 or G42 commands may be
programmed in a circular block to change cutter compensation direction
either left (G41) or right (G42).