Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 591)

Using Pocket Milling Cycles
Chapter 22
22-19
Use the G88.2 pocket milling finishing cycle to finish a circular pocket in a
workpiece. This cycle is typically used to remove the finish allowance that
was left on the sides of a circular pocket during a G88.1 cycle.
The G88.2 block used to finish a circular pocket has this format:
G88.2 X__Y__Z__R__P__H__L__F__;
Where : Is :
X Y The coordinates that specify the center of the circular pocket.
Z The coordinate (along the plunging axis) that specifies the bottom of the circular
pocket.
R The radius of the circular pocket. This parameter must be programmed.
P Direction of finishing cut.
H Finish allowance.
L Incremental plunge depth.
F Finishing feedrate.
In a finishing cycle, a smooth entry to and exit from the finish contour is
accomplished by having the tool approach and leave the finish contour
along a tangential arc. The radius of this arc is set equal to the tool radius
by the control. The tangential entry/exit point will always be at the left
side of the circular pocket along the -X axis.
Figure 22.7
Circular Pocket Finishing Using G88.2
TANGENTIAL
ENTRY/EXIT
PATH
(X, Y)
FINISH CUT
TOOL
RADIUS
Y
X
22.2.2
Circular Pocket Finishing
Using G88.2