As we begin 2021, we have found ourselves in a situation where our lead-times have substantially increased due to COVID-19 pandemic-related issues.
Those issues combined with high demand and heavy shipping volume is resulting in a longer than normal delivery timeframes for many Tormach machines and accessories.
We are working diligently to resolve these issues and look forward to bringing our lead-times back to normal. Unfortunately, this is going to take some time.
As of now, we anticipate that these lead times will continue into the second quarter. We appreciate your patience during this time.


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