The feed is locked to the thread
In rigid tapping the spindle and the Z axis turn and move together. One spindle revolution advances the tap exactly one thread pitch. So the feed is fixed:
Feed = pitch × RPM.
M6 × 1.0 tap at 500 RPM → F500. M10 × 1.5 at 400 RPM → F600. Imperial: feed = RPM ÷ TPI. Change the RPM and the feed changes with it. The pitch stays in charge.
What G84 actually does
One line, five moves:
- Rapid to the hole in XY.
- Rapid down to the R plane.
- Feed to depth, spindle forward, feed locked to the pitch.
- Reverse the spindle at the bottom.
- Feed back out to R. The tap unwinds along its own thread.
Then G98 or G99 sets the retract level, same as any drilling cycle. G74 is the mirror image for
left-hand threads.
Every hole pays the feed twice
The tap is screwed into the part at the bottom of the hole. The only way out is backwards along the thread with the spindle reversed, still locked to the pitch, still at feed. So a 15 mm thread at F500 costs 1.8 s of feed motion per hole before you count anything else.
Add the reversal. The spindle stops dead and spins up the other way, twice per hole (bottom and top). On most machines that’s around a second each time. Small number, big multiplier: forty tapped holes is over a minute of pure spindle reversal.
Put it on the clock
UltraNC runs G84 and G74 in full: feed in, reversal pause at the bottom, feed out, retract. Set your machine’s tool change time and the reversal is derived from it automatically. Load your file, and every tapped hole lands on the clock at its true cost, alongside the rapids, tool changes and dwells around it.
Common questions
How do I calculate the feed rate for tapping?
Feed = thread pitch × spindle RPM. An M6 tap has a 1.0 mm pitch, so at 500 RPM the feed is 500 mm/min. Imperial taps use feed = RPM ÷ TPI. The spindle and Z axis are locked together in rigid tapping, so this number isn't a choice. It comes straight from the geometry of the thread.
What is the difference between G84 and G74?
Direction. G84 is right-hand tapping: spindle forward on the way in, reversed on the way out. G74 is the left-hand version for left-hand threads. Motion and timing are the same, mirrored.
Why does the tap feed out instead of rapiding out?
Because it's screwed into the part. The tap must unwind along the thread it just cut (spindle reversed, Z synchronised) at the same pitch-locked feed. Rapiding out would rip the thread and snap the tap. So every tapped hole pays the feed twice: once in, once out.
How much time does tapping add per hole?
Twice the thread depth at the tapping feed, plus the spindle reversal at the bottom, plus the rapids between holes. Example: 15 mm deep at 500 mm/min is 1.8 s in-and-out, plus a reversal of a second or so. Across a plate of holes it adds up fast. Simulate the file to see the real total.
Part of the guide: How to estimate CNC machining time from G-code
The drilling cousins: Peck drilling and cycle time: G83 vs G73
The dead time between holes: Non-cutting time