Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 655)

Milling Fixed Cycles
Chapter 26
26-23
7. The cutting tool is then retracted at a rapid feedrate to the initial point
level as determined by G98.
When the single block function is active, the control stops axis motion
after steps 1, 2 and 7.
This cycle is used to cut right-handed threads. The format for the G84
cycle is as follows:
G84X__Y__Z__R__P__F__L__;
Where : Is :
X,Y specifies location of the hole.
Z defines the hole bottom.
R defines the R point level.
P defines the dwell period at hole bottom.
F defines the tapping feedrate. This should be programmed as close as possible
to the rate in which the tap will be moving into the part (calculated from the tap
thread pitch and the active spindle speed). Enter the feedrate in either IPM or
IPR modes. No special spindle synchronization occurs with this cycle.
L defines the number of times the milling fixed cycle is repeated.
(See section 26.3 for a detailed description of these parameters.)
CAUTION: The programmer or operator must set the direction
of spindle rotation for tap-in. The control forces the proper
spindle direction for the tap-out, but uses the programmed
spindle direction for the tap-in.
Important: When programming and executing a G84 tapping cycle,
consider this:
The programmer or operator must start spindle rotation.
Override usage - the control ignores the feedrate override switch and
clamps override at 100 percent.
During tapping the feedrate override switch, and the feedhold feature
are both disabled. Cycle stop is not acknowledged until the end of the
return operation.
(G84): Right-Hand Tapping
Cycle