Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 588)

Using Pocket Milling Cycles
Chapter 22
22-16
These features are prohibited during execution of pocket milling cycles:
MDI mode
Tool offset changes through the offset softkey
The following subsections cover using the G88.2 finishing cycle for each
of the possible pockets.
Use the G88.2 pocket milling finishing cycle to finish a rectangular pocket
in a workpiece. This cycle is typically used to remove the finish allowance
that was left on the sides of a rectangular pocket during a G88.1 roughing
cycle.
The G88.2 block used to finish a rectangular pocket has this format:
G88.2 X__Y__Z__I__J__(,R or ,C)__P__H__L__F__;
Where : Is :
X Y The coordinates that specify the center of the rectangular pocket.
Z The coordinate (along the plunging axis) that specifies the bottom of the
rectangular pocket. In incremental mode this parameter specifies the depth of
the pocket as measured from the start level to the pocket bottom. This
parameter must be programmed.
I J The length of the 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.
,R Corner radius. This is an optional parameter that is used to program rounded
interior corners in the rectangular pocket.
,C Corner chamfer. This is an optional parameter that is used to program
chamfered interior corners in the rectangular pocket.
Important: In order to program rounded or chamfered corners the
Chamfering and Corner Radius option must be installed in the control.
P Direction of finishing cut. This parameter determines whether the finishing cuts
are performed in a clockwise or counter-clockwise motion. P0 specifies
clockwise. P1 specifies counter-clockwise.
Important: Cutter compensation (G41/G42) must be disabled prior to the
G88.2 block. The control generates an error if compensation is not disabled.
H The finish allowance that will be left on the sides of the pocket. This is an
optional parameter that is provided to allow for multiple finishing cuts.
L Incremental plunge depth of each cutting pass plunge 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.
F Finishing feedrate. If not programmed the existing (modal) feedrate will be used.
22.2.1
Rectangular Pocket
Finishing Using G88.2