Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 601)

Using Post Milling Cycles
Chapter 23
23-7
If L is programmed, the tool plunges along the Z axis to the incremental
depth specified by the L parameter. If L is not programmed, the tool
plunges along the Z axis to the pocket depth specified by the Z parameter.
This move takes place at the plunge feedrate specified by the E parameter.
If E is not programmed, the plunge takes place at the roughing feedrate.
After the plunge operation, the control moves the tool in a circular path
that starts and ends at the same point on the -X axis. After completing a
circular path, the control makes a single-axis rough cut towards the post
along the -X axis. Another circular path is cut that start and ends at the -X
axis. This process is repeated until the sides of the pocket, less the finish
allowance H, are reached.
The width of the first roughing cut is equal to the tool radius. 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.
The tool is then simultaneously raised by the clearance amount and moved
at rapid feedrate along the -X axis back to the plunge-position. This
completes the machining of one L level.
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 programmed Z depth is reached.
Once the post has been machined out, the control simultaneously raises the
tool to the initial Z level while moving it away from the side of the post by
the clearance amount. This simultaneous move takes place at the rapid
feedrate. The tool is then moved at rapid feedrate along the X, Y, and Z
axes to the pre-cycle position of the tool.
Use the G88.4 post milling finishing cycle to remove the finish allowance
left on the sides of a rectangular or circular post. You can use this cycle to
finish a post formed by using a G88.3 roughing cycle. Typically a tool
change is made between the G88.3 and the G88.4 cycles.
Important: 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.
23.2
Post Milling Finishing Cycle
(G88.4)