Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 577)

Using Pocket Milling Cycles
Chapter 22
22-5
If ,R or ,C is not programmed in the G88.1 block, each corner of the
rectangular pocket is squared off as much as the tool radius will allow. If
,R or ,C is programmed in the G88.1 block, the corners of the rectangular
pocket will either be rounded or chamfered. Refer to chapter 16, Using
Chamfers and Corner Radius, for additional information on chamfers and
corner rounding.
Use the G88.1 pocket milling roughing cycle to enlarge an existing
rectangular pocket in a workpiece. This cycle makes multiple rectangular
cuts at a programmed width and depth.
The G88.1 block used to enlarge an existing rectangular pocket has this
format:
G88.1 X__Y__Z__I__J__Q__(,R or,C)__P__H__D__L__E__F__;
Where : Is :
X Y The coordinates that specify the center of the original rectangular pocket.
Z The coordinate (along the plunging axis) that specifies the bottom of the
rectangular pocket.
I J Length of the original rectangular pocket’s sides. I specifies the length of the side
parallel to the X axis. J specifies the length of the side parallel to the Y axis.
These are unsigned incremental values.
Important: It is assumed that I and J are assigned in AMP as the integrand
axis names that correspond to the X and Y axes respectively.
Q Unsigned incremental value that specifies how much the original rectangular
pocket should be enlarged. I and J are both enlarged by this amount.
,R Corner radius.
,C Corner chamfer.
P Direction of roughing cut.
H Finish allowance.
D Roughing cut thickness.
L Incremental plunge depth.
E Plunge feedrate.
F Roughing feedrate.
Important: The rectangular pocket does not have to be parallel to the axes
of the selected plane. It may be rotated by rotating the work coordinate
system (G68). Refer to chapter 13 for additional information on rotating
the work coordinate system.
22.1.2
Rectangular Pocket
Enlarging Using G88.1