Introducing the new 1500MX CNC Mill. Learn more



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

N50 G54

N55 M8

N65 G0 X0.5 Y-0.75

N70 G43 Z0.6 H51

N80 G0 Z0.2

N85 S400

N90 G98 G84 X0.5 Y-0.75 Z-0.605 R0.2 F20.

N95 X1.0 Y -1.25

N100 G80

N105 G0 Z0.6