Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 617)

Thread Cutting
Chapter 25
25-17
When this cycle is executed:
1. The cutting tool rapids to the depth programmed with the X-word.
2. The thread cutting pass is made to the position programmed with the
Z-word using a feedrate that generates the required lead programmed
with the E- or F-word. If the Thread Chamfering feature was enabled
before the cycle began executing, the control performs a chamfer just
before reaching the programmed Z position.
3. The cutting tool is retracted away from the part at a rapid feedrate to
where the X axis was positioned prior to the G21 block.
4. The cutting tool is returned along the Z axis at a rapid feedrate to
where the Z axis was positioned prior to the G21 block.
5. Program execution continues on to the next block.
G21 works like most fixed cycles in that it automatically repeats after
every rapid move until canceled. Following passes need only contain a
new value for the infeed (X value). The other parameters programmed in
the G21 block remain in effect.
Example 25.5
G21 Straight Thread Cutting Cycle
G00X10.Z10.; Rapid to the start point of the thread cutting cycle. This should be
a point that allows a straight, rapid, X move to the depth that the
thread is cut to.
S500.M03; Starts the spindle turning at 500 RPM in the clockwise direction.
G21X4.8Z5.F.5; This block makes a thread cutting pass with a lead of .5 and
return the cutting tool to the start point of the thread cutting cycle
(X10 Z10).
X4.5; This block repeats the G21 thread cutting block using a new
depth of cut to 4.5.
X4.3; This block repeats the G21 thread cutting block using a new
depth of cut to 4.3.
G00; This block cancels the G21 thread cutting mode.