Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 587)

Using Pocket Milling Cycles
Chapter 22
22-15
After completing the 360 degree circular path, the control makes a
single-axis rough cut outwards along the -X axis then cuts another 360
degree circular path. This process is repeated until the sides of the pocket,
less the finish allowance H, are reached. The tool is then simultaneously
raised by the clearance amount and moved at rapid feedrate back to the
plunge-position. This completes machining of one L level.
The width of the last roughing cut is equal to the tool radius plus the finish
allowance (H + TR). The width of the remaining roughing cuts is
calculated by the control based on the remaining area to be roughed-out
and the programmed rough cut thickness, D. The control divides the
remaining area by D to calculate the number of roughing cuts needed to
rough out this area. The control then adjusts the width and number of
these cuts until an even number of roughing cuts is achieved. The width of
these cuts will always be equal to or less than the programmed rough cut
thickness, D.
If the programmed Z depth of the pocket has not been reached, another
plunge along the Z axis to the next L level takes place. This level is then
machined as described in the previous paragraphs. This process is repeated
until the pocket is machined out.
Once the pocket has been machined out, the control simultaneously raises
the tool to the initial Z level plus the clearance amount while moving it
away from pocket edge by the clearance amount. This simultaneous move
takes place at the rapid feedrate. The tool is then moved at rapid feedrate
simultaneously along the X, Y, and Z axes to the pre-cycle position of the
tool.
Use the G88.2 pocket milling finishing cycle to remove the finish
allowance left on the sides of the rectangular or circular pockets, and slots.
Use this cycle to finish a pocket formed by using a G88.1 roughing cycle.
Typically a tool change is made between the G88.1 and the G88.2 cycles.
Important: Remember:
the active plane is selected using G17, G18, or G19
In this chapter it is assumed that G17, the XY plane, is selected as the
active plane.
tool length and diameter offsets must be entered and active prior to the
G88 block
if the radius of the finishing tool is larger than the radius of the roughing
tool, some material may be left in the corners of the pocket after the
finishing pass
22.2
Pocket Milling Finishing
Cycle (G88.2)