We use technical and security cookies and, only if you accept, analytics with no cross-site tracking. More in the Cookie policy and Privacy policy.
We use first-party cookies and technical storage to make the site work, Google reCAPTCHA security technology and, only if you accept, Vercel analytics (no cookies, no cross-site tracking). You can accept or reject analytics; both options are equivalent and you can change your choice at any time. More info: Cookie policy, Privacy policy, Legal notice and Terms and conditions.
G83 drills in several pecks: it goes down Q millimeters at feed, pulls out in rapid to the R plane to drop the chips, rapids back in to just short of where it stopped and carries on, until it reaches the Z bottom. It is the cycle for holes deeper than three or four diameters and for materials that make stringy chips. Q is always positive and incremental: it is the depth of each peck, not a coordinate.
For reference only: syntax changes with the control, the post-processor and the machine parameters. Check the official manual and run a simulation before cutting. Legal notice.
Fanuc (milling)
G99 G83 X30. Y20. Z-60. R2. Q8. F110The gap the control leaves when it comes back in (the rapid approach distance before it picks the cut up again) is a machine parameter, not something you program. The G73 variant does the same thing but with a short retract inside the hole.
Haas (milling)
G99 G83 X30. Y20. Z-60. R2. Q8. F110Haas also accepts I (first peck), J (how much each peck is reduced) and K (minimum peck) instead of Q, to shorten the peck as the hole gets deeper. Setting 52 decides whether the retract reaches the R plane or stops above it.
Siemens 840D / 828D
CYCLE83(RTP, RFP, SDIS, DP, DPR, FDEP, FDPR, DAM, DTB, DTS, FRF, VARI)The CYCLE83 parameters are positional. The one that decides the behavior is VARI: with chip breaking the retract is short (the equivalent of G73) and with chip removal the drill comes out of the hole (the equivalent of G83).
Heidenhain TNC (Klartext)
CYCL DEF 203 TALADRADO UNIVERSALIn cycle 203, Q202 is the plunging depth of each peck and Q212 is how much it is reduced on each one. Cycle 205 adds chip breaking, a sunk starting point and a relief, for very deep holes.
| Letter | What it sets | Unit |
|---|---|---|
| X Y | Hole position. Every new block with an X or a Y repeats the whole cycle, pecks included. | mm / in |
| Z | Hole bottom: absolute dimension under G90, distance from the R plane under G91. | mm / in |
| R | Reference plane. It matters twice as much in G83 as in G81, because the drill comes up to it on every peck: a high R multiplies cycle time. | mm / in |
| Q | Depth of each peck. Always positive and incremental; it is not a coordinate and it is not the total depth. | mm / in |
| F | Drilling feedrate. Modal: leave it out and the last F in the program is inherited. | mm/min under G94 |
| K / L | Cycle repeats in incremental mode (K on Fanuc, L on Haas) for rows of evenly spaced holes. | integer |
Two 10 mm holes 60 mm deep, six diameters, in carbon steel with an HSS-Co drill. It pecks 8 mm at a time so the chips clear; with a cycle that does not peck at that depth the drill packs up. The points were already spotted with a spot drill in the previous operation.
G91 G28 Z0. | ( Z to the reference point in incremental before the change. ) |
T7 M06 | ( 10 mm HSS-Co drill. ) |
G90 G54 G00 X30. Y20. | ( Absolute, work offset and rapid over the first hole. ) |
G43 H07 Z50. M03 S900 | ( T7 length offset and spindle at 900 rpm, around 28 m/min of cutting speed on 10 mm. ) |
M08 | ( Coolant on. At six diameters it is not optional. ) |
G99 G83 Z-60. R2. Q8. F110 | ( Eight pecks: 8 mm down at feed, out in rapid to Z2, back in and repeat down to Z-60. Q8 is incremental and positive; the 110 mm/min feed works out at about 0.06 mm per tooth. ) |
X90. | ( Second hole: the whole cycle repeats with the same pecks. ) |
G80 G00 Z50. M09 | ( Cancels the cycle before any rapid move and turns the coolant off. ) |
G91 G28 Z0. M05 | ( Safe retract and spindle stop. ) |
G90 M30 | ( Back to absolute and end. ) |
As soon as the hole goes past three or four diameters the chips stop coming out on their own: they wrap up in the drill flutes, rub against the wall, and torque climbs until the drill packs up or snaps. G83 stops that because it pulls the drill out of the hole on every peck and the chips fall off. You also need it before that depth in materials that make long, gummy chips, such as low carbon steels or soft aluminum, and any time there is no through coolant pushing the chips out.
A reasonable starting point is a Q of one diameter for the first pecks and half a diameter from four or five diameters deep, because the deeper the drill is the further it has to drag the chips. On Fanuc the Q is a single value for the whole hole, so you pick the value for the worst stretch; on Haas you can step it down with I, J and K. Keep the R plane low, 2 or 3 mm, because the drill comes up to it on every peck and every extra millimeter is paid for times the number of pecks.
The control chains the pecks and, coming back in, approaches in rapid leaving a small gap before it picks the cut up again. That gap is a machine parameter and is not programmed, so you cannot take the exact value for granted. On Haas there is also a setting that decides whether the retract reaches the R plane or stops above the last peck. What you do control is the number of pecks, which comes out of dividing the depth by Q, and with it the cycle time and the life of the drill.
Each peck, and always positive and incremental. The total depth is the Z. With Z-60, R2 and Q8 the control makes eight 8 mm pecks down to the Z-60 coordinate.
G73 backs off only a few tenths or millimeters inside the hole: it breaks the chip but does not clear it, and it is fast. G83 pulls the drill out to the R plane on every peck: it is slower but it is the only thing that works past four or five diameters and in long chipping material.
As a starting point, one drill diameter for the first pecks and half a diameter from four or five diameters deep. If the hole gets long and the machine starts to sound different or the spindle load climbs, drop Q before you break the drill.
On Fanuc, yes: the retract goes all the way to the R plane. On Haas it depends on Setting 52, which can leave the retract above the last peck instead of clearing the hole. If the detail matters to you, check your machine manual before you rely on it.
Yes, but with other codes: some controls accept Q inside the G84 rigid tapping cycle, and Fanuc has G84.2 and G84.3 for peck tapping. It depends on the machine option, so check it before you run it with a tap down the hole.
CNC IDE: editing with G/M tooltips, line inspector, conversion between controls and 2D/3D toolpath.
CNC Alarms and Solutions Guide. Enter the error code or symptom to find the cause and how to repair it at the machine.
Estimate CNC turning and milling cycle time from G-code. Calculate parts per hour with a breakdown of cutting, rapids, canned cycles and tool changes.