Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 574)

Using Pocket Milling Cycles
Chapter 22
22-2
Use the G88.1 pocket milling roughing cycle to rough out a rectangular
pocket in a workpiece. This cycle makes multiple rectangular cuts at a
programmed width and depth.
The G88.1 block used to rough out a rectangular pocket has this format:
G88.1 X__Y__Z__I__J__(,R or,C)__P__H__D__L__E__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.
Important: When roughing out a rectangular pocket, the tool diameter can
not exceed the length of the shortest side of the rectangular pocket. If it does,
the control enters Cycle-Stop mode and displays the error message “TOOL
RADIUS TOO LARGE”on the CRT.
,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: Cutter compensation (G41/G42) must be disabled prior to the
G88.1 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 finish
allowance can be removed later using a G88.2 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 G88.2 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 current
tool diameter. If it is, the control will enter Cycle-Stop mode and display the error
message “D-WORD LARGER THAN TOOL DIAMETER”on the CRT.
L Incremental plunge depth of each cutting pass along the Z axis. If L is not
programmed, the plunge amount will be equal to the programmed depth of the
pocket. This is an optional parameter.
22.1.1
Rectangular Pocket
Roughing Using G88.1