Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 356)

Coordinate Control
Chapter 13
13-4
Note that in the preceding figure the center of rotation programmed in the
G68 block is ignored when the block immediately following the G68 is an
incremental motion block.
Angles and centers of rotation for G68 blocks are modal and remain in
effect for following G68 blocks until a new center of rotation or angle is
specified with a G68 command.
Important: It is possible to rotate all of the work coordinate systems at
once by using the external part rotation.
If rotating the coordinate system again in the same plane using another
G68 command:
while in incremental mode, the angle of rotation is taken from the
current rotated coordinate position (see Figure 13.3)
while in absolute mode, the angle of rotation is taken from the original
position
Rotating the coordinate system again in a different plane using another
G68 is not allowed.
Executing a G69 cancels all G68 rotations and returns the coordinate
system back to its original orientation. Local rotation of a work coordinate
system using the G68 command is also canceled when the control executes
an M30 or M02 code in a program.
Example 13.2
Multiple Rotation of the Coordinate System While in Incremental Mode
Program Block Comment
N01 G54 G91; Incremental mode
N02 G68X0Y0R10; Rotates the current work coordinate system 10 degrees.
N03 G68X5.Y4.R30; Rotates the current work coordinate system 30 degrees
about a center point of X5., Y4. for a total rotation from
its original position of 40 degrees.
N04 G69; Returns the work coordinate system to its original posi-
tion of 0 degrees.