Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 602)

Using Post Milling Cycles
Chapter 23
23-8
Important: Tool length, work coordinates, and diameter offsets must be
entered and active prior to the G88 block. The radius/diameter of the tool
can not exceed the length of the shortest side of the pocket. If it does, the
control enters Cycle-Stop mode and displays the error message “TOOL
RADIUS TOO LARGE.”
These features are prohibited during execution of pocket milling cycles:
MDI mode
Tool offset changes through the offset softkey
Work coordinate offset changes through the offset softkeys
The following subsections cover using the G88.4 finishing cycle for
rectangular or circular posts.
Use the G88.4 post milling finishing cycle to finish a rectangular post in a
workpiece. This cycle is typically used to remove the finish allowance that
was left on the sides of a rectangular post during a G88.3 cycle.
The G88.4 block used to finish a rectangular post has this format:
G88.4 X__Y__Z__I__J__Q__(,R or ,C)__P__H__L__F__;
Where : Is :
X Y The coordinates that specify the center of the rectangular post.
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 post’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 the distance from the sides of the post to the outer
perimeter of the pocket. This distance is the same whether measured along the X or the Y axis.
,R Corner radius. This is an optional parameter that is used to program rounded post corners.
,C Corner chamfer. This is an optional parameter that is used to program chamfered rounded post
corners.
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: If cutter compensation (G41/G42) was enabled prior to the G88.4 block, it is
disabled when G88.4 is enabled.
H The finish allowance that will be left on the sides of the post. This is an optional parameter that is
provided to allow for multiple finishing cuts.
23.2.1
Rectangular Post Finishing
Using G88.4