Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 646)

Drilling Cycles
Chapter 26
26-20
Use this cycle to cut right-handed threads.
The format for the G84.2 cycle is:
G84.2X__Z__R__F__L__Q__D__S__;
Where : Is :
X specifies location of the hole.
Z
defines the hole bottom.
R defines the R point level.
F defines the thread lead along the drilling axis (Z in this manual). It is mandatory
and modal in any subsequent solid tapping cycle blocks until a new F-word is
programmed.
The control interprets the F-word as the thread lead in inches per revolution or
millimeters per revolution, depending on the inch/metric mode active.
L defines the number of times the drilling cycle is repeated.
Q defines the angle at which to orient the spindle before starting the tap. It is modal
in any subsequent solid tapping blocks until a new Q-word is programmed or the
tapping cycle is cancelled by a G80. To retap a hole, a Q-word must have been
programmed when the hole was originally tapped.
D defines the return spindle speed, but cannot exceed the maximum tapping
spindle speed set in AMP. This will adjust your Z-axis feedrate according to the
thread lead defined in F.
S defines spindle speed in rpm.
See section 27.3 for a detailed description of these parameters.
Important: When programming and executing a G84.2 solid-tapping
cycle, remember:
the feedrate of the tapping phases is derived as
(spindle {RPM}
*
F-lead {IPR}) = IPM
the spindle speed that is active at the start of the cycle determines the
effective Z feedrate
the direction of spindle rotation for tap-in and tap-out phases will be
automatically generated by the control
spindle speed override has no effect on the solid-tapping cycle; you can
use feedrate override to adjust the tapping operation
D cannot exceed the maximum tapping spindle speed set in AMP
you cannot select tools via D-word while in solid-tapping mode
gear changes are locked out
(G84.2): Right-Hand
Solid-Tapping Cycle