Owner's manual

Milling Fixed Cycles
Chapter 26
26-23
7. The cutting t ool 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 i s used to cut right-handed threads. The format for the G84
cycle is a s follows:
G84X__Y__Z__R__P__F__L__;
Where : Is :
X,Y
specifieslocation ofthe hole.
Z
defines the holebottom.
R
defines the Rpointlevel.
P
defines the dwell period atholebottom.
F
defines the tapping feedrate. Thisshouldbe programmed ascloseas possible
to the rate inwhichthetap willbemovingintothe part(calculated fromthe tap
thread pitchand the active spindle speed). Enterthe feedrate ineither IPMor
IPR modes. No special spindle synchronization occurs with this cycle.
L
defines the numberoftimesthe millingfixedcycle isrepeated.
(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 c ontrol 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