Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 628)

Irregular Pocket Milling Cycles
Chapter 25
25-10
Use the irregular pocket milling finishing cycle (G89.2) to finish an
irregular pocket in a workpiece. This cycle is typically used to finish an
irregular pocket formed using a G89.1 irregular pocket roughing cycle. A
tool change is usually performed between the G89.1 and G89.2 cycles.
You can use this cycle to finish a post that was formed by combining two
pocket cycles.
The G89.2 block has this format:
G89.2 X__Y__Z__P__Q__H__F__L__;
Where : Is :
X Y The coordinates that specify the start/end corner of the irregular pocket in the
selected plane. These parameters must be programmed.
Z The coordinate (along the plunging axis) that specifies the bottom of the irregular
pocket. In incremental mode this parameter specifies the depth of the pocket as
measured from the start-point to the pocket bottom. This parameter must be
programmed.
P The sequence number of the first block in the set of blocks that define the pocket
shape. The coordinates in this block specify the start-point of the pocket’s first
wall. This start-point must correspond to the start/end corner specified by the X
and Y coordinates. This parameter must be programmed.
Q The sequence number of the last block in the set of blocks that define the pocket
shape. The coordinates in this block specify the endpoint of the pocket’s last
wall. This endpoint must correspond to the start/end corner specified by the X
and Y coordinates. This parameter must be programmed.
The set of blocks specified by P and Q may be located anywhere after the calling
block (even after an end of program command), as long as the calling block is in
the same program as the set of blocks. This means that blocks defining the
pocket shape can not be called from a subprogram or a macro unless the calling
block is in that subprogram or macro.
H The finish allowance that will be left on the sides of the irregular pocket. This is
an optional parameter that provides for multiple finishing cycles.
F Finishing feedrate. This parameter determines the feedrate of any XY axis
cutting moves. If not programmed the existing (modal) cutting feedrate will be
used.
L Incremental plunge depth of each cutting pass along the Z axis. If L is
programmed, a finish pass is made at each L level. If L is not programmed, only
one finishing pass is made at the programmed Z depth. This is an optional
parameter. It is typically programmed when a very deep pocket is being finished.
25.1.2
Irregular Pocket Finishing
(G89.2)