If you’ve ever seen “LH” on a print next to a threaded hole, you’ve found yourself a left-hand thread. They tighten counterclockwise instead of the usual way, and your standard G84 tapping cycle won’t cut them correctly.
That’s what G74 is for.
G74 is the left-hand tapping canned cycle. It runs the spindle in reverse, feeds down to depth, then reverses out — same basic idea as G84, just spinning the other direction. You’ll also use it for peck tapping when you need to clear chips out of a deep hole.
This page covers how G74 works, how to format it, and what to watch out for before you run it.
Key Takeaways
- G74 is the left-hand tapping canned cycle — it cuts threads that screw in the opposite direction of standard threads
- The spindle must be set to counterclockwise rotation with M04 before calling G74
- The feedrate (F) must equal the pitch of the thread — not a cutting speed
- Add the Q parameter to switch from rigid tapping to peck tapping
- Cancel with G80 when done, or the machine will attempt to tap every new position in the program
| G74 – At A Glance | |
|---|---|
| Function | Left-Hand Tapping Canned Cycle |
| Format | G98 G74 X__ Y__ R__ Z__ F__ |
| Type | Modal (Group 9) |
| Spindle direction | Counterclockwise (M04) |
| Cancelled by | G80 |
| Peck tapping | Yes — add Q parameter |
What does G74 do?
G74 activates the left-hand (reverse) tapping canned cycle on a CNC machining center.
Tapping creates internal threads — the kind that a bolt or screw gets threaded into. G74 specifically cuts left-hand threads, which are the opposite of standard threads. They tighten counterclockwise and loosen clockwise. Think lefty-tighty, righty-loosey.
When G74 runs, the spindle rotates counterclockwise (M04), feeds down to the programmed depth, reverses direction, and feeds back out. That’s the whole cycle.
Use G74 when the print calls for a left-hand thread. For standard right-hand threads, use G84 instead.
Parameters Used with G74
These are the words (addresses) that control how G74 runs:
- X, Y — Position of the hole to be tapped
- R — The R-plane (retract plane) — the Z height the tool clears to when moving between holes
- Z — Final tapping depth (bottom of the thread, not top)
- F — Feedrate — must equal the thread pitch
- Q — Peck depth (optional — only include if you want peck tapping)
- K or L — Number of times to repeat the cycle (machine-dependent)
- G98 or G99 — Controls where the tool retracts between holes (initial point vs. R-plane)
The R-plane should clear all clamps, fixtures, and part features. When tapping, set it a little higher than you normally would. The machine needs a moment to sync spindle speed and feedrate before the tool enters the hole.
Programming Format
The standard format looks like this:
G98 G74 X__ Y__ R__ Z__ F__In most programs, you’ll see the hole position on a separate line:
X2.0 Y3.0
G98 G74 R0.25 Z-1.5 F0.0625The program moves the tool to the hole location first, then calls the tapping cycle.
The Z value is the bottom of the thread — not the surface of the part. Don’t confuse it with the start of the hole.
Setting the Feedrate
The feedrate for tapping is not a cutting speed. It must equal the pitch of the thread.
For inch threads, pitch = 1 ÷ threads per inch.
- 1/4-20 thread → F = 1 ÷ 20 = 0.050 IPR (or IPM at the corresponding RPM)
- 5/16-18 thread → F = 1 ÷ 18 = 0.0556
For metric threads, the pitch is listed directly on the print.
- M10 x 1.5 → F = 1.5 mm/rev
Speeds and feed overrides are disabled during tapping for safety. The machine locks them out so you can’t accidentally change the ratio between spindle speed and feed — which would strip or break the tap.
Hole Prep Before Tapping
G74 requires a pre-drilled hole. Do not use it to drill and tap in one step.
The tap drill diameter = thread major diameter − pitch.
- M10 x 1.5 → tap drill = 10 − 1.5 = 8.5 mm
Drill the hole first with a standard drilling cycle (G81 or G83), then call G74.
COMMON MISTAKE – Wrong Spindle Direction
G74 requires M04 (counterclockwise) — not M03.
If you run G74 with the spindle turning clockwise, you’ll strip threads or break the tap immediately. Always confirm M04 is active before the G74 block runs. This is the single most common G74 setup error.
G74 Rigid Tapping
Rigid tapping means the spindle and the Z-axis feed are electronically synchronized — the machine treats the tap like a leadscrew. There’s no floating tap holder needed.
Not all machines support rigid tapping. On Fanuc-based controls, it’s typically enabled with M29 before the G74 call:
M29 S500
G98 G74 X2.0 Y3.0 R0.25 Z-1.5 F0.0625Check your machine’s parameter settings and manual to confirm rigid tapping is enabled. On older machines, you may need a tension-compression tap holder instead.
Rigid tapping is fast and accurate, but it can run into trouble with chip buildup in deep holes or tough materials. That’s where peck tapping helps.
G74 Peck Tapping
Adding the Q parameter to G74 switches it to peck tapping mode. The tap feeds in to the Q depth, retracts partially to break chips, then feeds deeper — one peck at a time until it reaches the Z depth.
G98 G74 X2.0 Y3.0 R0.25 Z-1.5 Q0.25 F0.0625This example pecks in 0.25″ increments.
Peck tapping is slower than rigid tapping, but it keeps chips from packing into the hole. Use it for deep threads, small taps, or sticky materials like aluminum.
G84 vs. G74
G84 is the standard right-hand tapping cycle. G74 is the left-hand version.
The only real difference: G84 uses M03 (clockwise spindle), G74 uses M04 (counterclockwise). The formats are otherwise identical.
| G84 | G74 | |
|---|---|---|
| Thread type | Right-hand (standard) | Left-hand (reverse) |
| Spindle | M03 — clockwise | M04 — counterclockwise |
| Tightens | Clockwise | Counterclockwise |
| Peck capable | Yes (Q) | Yes (Q) |
Both are modal — they stay active until you cancel with G80.
Canceling G74
Cancel the cycle with G80:
G80If you forget G80, the machine will attempt to tap a hole at every new X/Y position in the program. That’s a bad day. Always cancel your canned cycles before moving on.
G74 code example
G00 X50.0 Y50.0 (Rapid to first hole location)
M04 S500 (Spindle on counterclockwise at 500 RPM)
G98 G74 R5.0 Z-40.0 F1.5 (Left-hand tap, 40mm deep, 1.5mm pitch)
X25.0 (Tap second hole at X25, Y50)
Y25.0 (Tap third hole at X25, Y25)
G80 (Cancel canned cycle)
Z10.0 (Retract Z)
M30 (End program)The tool taps three holes in sequence. G98 returns the Z to the initial point between moves. G80 ends the cycle after the last hole.
FAQs
What is G74 used for?
G74 is used to cut left-hand internal threads in a pre-drilled hole. It’s the reverse tapping canned cycle — the spindle runs counterclockwise to cut threads that tighten counterclockwise.
What’s the difference between G74 and G84?
G84 cuts standard right-hand threads with a clockwise spindle (M03). G74 cuts left-hand threads with a counterclockwise spindle (M04). The programming format is otherwise the same.
How do I set the feedrate for G74?
The feedrate must equal the pitch of the thread. For metric threads, use the pitch number directly (M10x1.5 → F1.5). For inch threads, divide 1 by the threads per inch (1/4-20 → F0.050).
Do I need to drill a hole before using G74?
Yes. G74 only cuts threads — it does not drill. Always run a drilling cycle (G81 or G83) with the correct tap drill size before calling G74.