Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 543)

Single-Pass Turning Cycles
Chapter 22
22-3
CAUTION: When programming the single-pass cycle, the first
move to the depth of cut is a rapid move. Make sure that the
tool does not contact the part on this initial move.
The feedrate used in the single-pass cycle is the currently active
programmed cutting feedrate. If desired, a different cutting feedrate may
be specified in the single-pass cycle block.
The rapid feedrate (for the axis in motion as assigned in AMP) is used for
the approach to the part and the return to start point.
G20 Straight O.D. and I.D. Roughing
The format for the G20 straight cutting cycle is as follows:
G20X__ Z__;
Where : Is :
X__ is the depth of cut for the X axis. In incremental mode, specify the amount of
infeed. In absolute mode, specify the coordinate position at the desired depth of
cut. X may be programmed as either a diameter or radius value.
Z__ is the length of cut along the Z axis. In incremental, specify the amount of feed
across the part. In absolute, specify the coordinate position of the end point of the
cutting stroke.
After the G20 block is executed, the control re-executes the cycle for any
following block that commands axis motion (until the cycle is cancelled).
The value of the axis word in that block is used to replace the parameter
determined with that axis word in the original G20 block and the cycle is
re-executed using these new parameters.