TAPPING CYCLE (G84)
The G84 cycle is intended for tapping. This cycle rotates the spindle clockwise to tap a pre-drilled hole; when the bottom of the hole is reached, the spindle rotates in the reverse direction and exits the hole.
Program: G84 X~ Y~ Z~ R~ P~ F~
- P~ is the number of seconds to dwell
- F~ is the feed rate
The G84 cycle is as follows:
- Step 1: Preliminary canned cycle motion.
- Step 2: Start the spindle forward.
- Step 3: Move the Z-axis at the programmed feed rate (F~) to the Z-depth.
- Step 4: Reverse the spindle.
- Step 5: Dwell for the P number of seconds.
- Step 6: Retract the Z-axis at the programmed feed rate (F~) to the R-plane.
This cycle uses a P word, where P specifies the number of seconds to dwell. The P word is optional – if it is not included, PathPilot calculates a dwell for you (half of a second per 1000 RPM).
Spindle speed must be commanded before calling a G84 cycle. Feed rate override is ignored during a tapping cycle. Feedhold is ignored until the return operation is executed. After the tapping operation is completed, either a G98 or G99 command controls the return height — G99 returns the tool to the R-plane; G98 returns the tool to the initial height.
Example code using G84cycle:
N40 T51 G43 H51 M6
N45 S400 M3
N65 G0 X0.5 Y-0.75
N70 G43 Z0.6 H51
N80 G0 Z0.2
N90 G98 G84 X0.5 Y-0.75 Z-0.605 R0.2 F20.
N95 X1.0 Y -1.25
N105 G0 Z0.6