Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 596)

Using Post Milling Cycles
Chapter 23
23-2
Use the G88.3 post milling roughing cycle to rough out a rectangular post
in a workpiece. This cycle makes multiple cuts at a programmed width
and depth.
The G88.3 block used to rough out a rectangular post has this format:
G88.3 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 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 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 roughing cut. This parameter determines whether the roughing 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 G88.3 block, it is
disabled when G88.3 is enabled.
H The finish allowance that will be left on the sides of the post. This finish allowance can be removed
later using a G88.4 finishing cycle.
To leave a finish allowance on the pocket bottom, program a pocket depth (Z parameter) that is at
the desired finish allowance above the actual pocket bottom. This finish allowance can be removed
later using a G88.4 finishing cycle.
D Roughing cut thickness. This parameter specifies the maximum width of any XY axis roughing
cuts. This is an optional parameter. If not programmed, the control uses the default thickness,
which is equal to half of the current tool diameter.
Important: The roughing cut thickness can not be greater than the diameter of the current
tool. If it is, the control enters Cycle-Stop mode and displays the error message “D-WORD
LARGER THAN TOOL DIAMETER”on the CRT.
L Incremental plunge depth of each cutting pass along the Z axis. This is an optional parameter. If
not programmed, the plunge amount will be equal to the programmed depth of the pocket.
E Plunge feedrate. This parameter determines the feedrate of any Z axis moves. If not programmed
the roughing feedrate (F) will be used.
F Roughing feedrate. This parameter determines the feedrate of any XY axis moves. If not
programmed the existing (modal) feedrate will be used.
23.1.1
Rectangular Post Roughing
Using G88.3