Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 636)

Milling Fixed Cycles
Chapter 26
26-4
This section assumes that the programmer can determine the hole
machining axis using the plane select G--codes (G17, G18, and G19).
Refer to the system installer’s documentation to make sure that a specific
axis has not been selected in AMP to be the hole machining axis.
G--codes, G17, G18 or G19, determine the plane, the positioning axes and
the hole machining axis. The two axes that define the selected plane are
used as positioning axes; the axis perpendicular to the plane is the hole
machining axis.
Table 26.B below assumes that the system installer has not altered the
default values defining the G17, G18 or G19 plane select codes.
Table 26.B
Plane Selection vs Machining Axis
Plane Hole Machining Axis Positioning Axes
XY (G17) Z axis or its parallel axis X and Y axes or their parallel axes
ZX (G18) Y axis or its parallel axis Z and X axes or their parallel axes
YZ (G19) X axis or its parallel axis Y and Z axes or their parallel axes
Example 26.1 shows you how to change the hole machining axis to a
parallel axis. A G80 should be executed to cancel any active milling
mode, prior to changing the hole machining axis.
Example 26.1
Altering the Machining Axis to a Parallel Axis
Program Block Comment
The W axis is parallel to the Z axis.
G17; XY plane active
G81X ___ Y ___ ; Drilling cycle, Z is the hole
machining axis
.
.
G80; Cancel milling cycle mode
G81X ___ Y ___ W ___; Drilling cycle, W is the hole
machining axis
.
.
. W must be programmed in every
subsequent block to remain the
drilling axis. If it is not
programmed, Z becomes the
drilling axis.
26.2
Positioning and Hole
Machining Axes