What is the difference between G81 and G83?

G81 plunges to depth in one continuous feed — right for shallow holes. G83 pecks: it drills a Q-depth increment, retracts fully to the R plane to clear chips, and re-enters, repeating to depth. Use G83 when the hole is deeper than roughly 3–4 tool diameters.

What do R, Z and Q mean in a drilling cycle?

R is the retract plane — the height the tool rapids to before feeding, and returns to between pecks. Z is the final hole depth. Q is the peck increment for G73/G83, always given as a positive incremental distance.

What is the difference between G98 and G99?

They set where the tool retracts after each hole (on a mill): G98 returns to the initial Z — the height before the cycle started — while G99 returns only to the R plane. G99 is faster between holes on a flat part; G98 clears clamps and steps. Warning: on a FANUC lathe, G98/G99 mean feed-per-minute/per-revolution instead.

Why doesn't G81 work on my GRBL machine?

GRBL has no canned cycles at all. CAM posts for GRBL expand each hole into explicit G0/G1 moves. If a file full of G81s runs strangely on GRBL, it was posted for the wrong control.

G81, G82, G83: Drilling Canned Cycles Explained

Canned cycles compress the whole drill-a-hole dance — rapid over, rapid down to clearance, feed to depth, retract — into one line per hole. After a cycle block, every following coordinate line drills another hole with the same parameters:

G90 G17 G54
G0 X10 Y10          ; over the first hole
G81 R2 Z-12 F150    ; drill it: rapid to Z2, feed to Z-12, retract
X30                 ; second hole — same cycle repeats
X50 Y25             ; third
G80                 ; cancel the cycle mode

The family shares the same block shape and differs in what happens at the bottom of the hole:

G81 — feed to depth, rapid out. Plain drilling.
G82 — dwell (P, in seconds/ms per control) at the bottom, then out. Flat-bottom spots and counterbores.
G83 — peck: feed down Q, rapid all the way out to R to clear chips, rapid back, repeat. Deep holes.
G73 — high-speed peck: short chip-breaking retract instead of a full one. Faster, for materials that chip well.
G84 / G74 — right/left tapping (spindle reverses at depth); rigid-tap variants are control-specific (LinuxCNC G33.1, Mach4 G84.2/.3).
G85 / G89 — boring: feed out instead of rapid, for finish bores.
G80 — cancel; the axis words go back to meaning normal moves.

Operation	LinuxCNC	GRBL	Centroid	FANUC	Mach3	Mach4	Notes
Cancel canned cycle	`G80`	—	`G80`	`G80`	`G80`	`G80`	Required to exit drill/bore/tap modes.
Standard drilling	`G81`	—	`G81`	`G81`	`G81`	`G81`	Z down at feed, rapid out.
Drilling with dwell at bottom	`G82`	—	`G82`	`G82`	`G82`	`G82`	Spot / counterbore use.
Peck drilling (full retract)	`G83`	—	`G83`	`G83`	`G83`	`G83`	Q = peck depth; full retract clears chips.
High-speed peck drilling (short retract)	`G73`	—	`G73`	`G73`	`G73`	`G73`
Right-hand tapping	`G84`	—	`G84`	`G84`	`G84`	`G84`	Mach3: needs OEM plugin for rigid tap
Left-hand / counter tapping	`G74`	—	`G74`	`G74`	`G74`	`G74`	FANUC LATHE reassigns G74 to a face-grooving cycle — see false friends.
Rigid tapping	`G33.1`	—	—	—	—	`G84.2` / `G84.3`	Dedicated rigid-tap codes; otherwise rigid mode is a flag on G84. LinuxCNC: LinuxCNC rigid-tap code
Boring (feed in, feed out)	`G85`	—	`G85`	`G85`	`G85`	`G85`
Boring with dwell (feed out)	`G89`	—	`G89`	`G89`	`G89`	`G89`
Return to initial Z after a cycle	`G98`	—	`G98`	`G98`	`G98`	`G98`	FANUC LATHE reassigns G98 to feed-per-minute — see the Turning group and false friends.
Return to R-plane after a cycle	`G99`	—	`G99`	`G99`	`G99`	`G99`	FANUC LATHE reassigns G99 to feed-per-revolution.

— means the control has no equivalent code. Full cross-control tables: the complete G-code & M-code reference.

R planes and retract modes

Two heights govern every cycle: the initial Z (where the tool was when the cycle block executed) and the R plane (R word — the feed-start / retract height just above the part). G98/G99 choose which one the tool returns to between holes:

G0 Z25              ; initial Z: above the clamps
G99 G83 R2 Z-30 Q5 F120   ; pecks; retracts only to Z2 between holes
X40                 ; fast hole-to-hole moves at Z2
G98 X70             ; this hole retracts to Z25 — clearing the clamp
G80

Watching a peck cycle in a simulator makes the R-plane logic obvious in a way no manual page does — each peck's full retract, the G99 skim moves, the one G98 hole that pops up high.

Common mistakes

Forgetting G80. The cycle is modal; an X line meant as a positioning move after the "last" hole cheerfully drills one more where it lands.
R plane below the part surface. The rapid-to-R move becomes a rapid into material. R sits just above the stock — 1–3 mm is typical.
Q as an absolute depth. Peck increments are positive and incremental. Q5 means 5 per peck, not "peck at Z-5".
G99 under a clamp. Retracting only to the R plane is quick until the hole-to-hole path passes under a strap clamp at Z2. Switch to G98 for holes with obstacles between them.
Expecting cycles on GRBL. Not there — post for the target control.

G81, G82, G83: Drilling Canned Cycles Explained

R planes and retract modes

Common mistakes

Frequently asked questions

See it, don't guess it

G81, G82, G83: Drilling Canned Cycles Explained

#R planes and retract modes

#Common mistakes

Frequently asked questions

Related G-code guides

See it, don't guess it

R planes and retract modes

Common mistakes