Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 613)

Using Hemisphere Milling Cycles
Chapter 24
24-7
With a convex hemisphere, the plunge is actually a contour move to the
outward along the -X axis. This move cuts along the spherical contour,
axes X and Z, at the plunge feedrate specified by the E parameter. This
plunge simultaneously moves the X and Z axes by the D’and L’amounts.
After the plunge, the control moves the tool in a 360 degree circular path
around the plunge-position. After completing this circular path, the control
makes a rough cut, D parameter, outwards along the -X axis. Another 360
degree circular path is cut that ends at the -X axis. This process is repeated
until the outer diameter of the pocket, plus the finish allowance H, is
reached. The tool is then raised by the clearance amount and moved at
rapid feedrate back to the initial cut at the current level. This completes
machining of one L level.
Important: The outer diameter of the pocket is equal to the radius of the
hemisphere plus the tool diameter and the finish allowance.
If the programmed Z depth of the pocket has not been reached, another
plunge takes place simultaneously along the X and Z axes to the next L’
level. This level is then machined as described in the previous paragraphs.
This process is repeated until the programmed Z depth of the convex
hemisphere is reached, at which time the tool is moved at rapid feedrate
along the Z axis back to the initial Z level. The tool is then moved at rapid
feedrate along the X and Y axes to its pre-cycle position.
Use the G88.6 hemisphere milling finishing cycle to remove the finish
allowance left on the sides of a concave or convex hemisphere. You can
use this cycle to finish a hemisphere formed by using a G88.5 roughing
cycle. Typically a tool change is made between the G88.5 and the G88.6
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.
Important: Tool length and diameter offsets must be entered and active
prior to the G88 block.
These features are prohibited during execution of pocket milling cycles:
MDI mode
Tool offset changes through the offset softkey
24.2
Hemisphere Milling
Finishing Cycle (G88.6)