The G83 peck drilling cycle: understanding Q infeed, the R point and G98/G99 return levels
Explains the G83 peck drilling cycle of machining centers with a three-hole example: Q infeed and chip evacuation, the difference between the R point and the initial point, choosing G98 or G99 return, the difference from G73, and how the meaning of R changes in lathe G83.
Why drills break in deep holes
The deeper a drill goes, the further the chips have to travel up its narrow flutes. Once the hole depth starts to exceed three times the drill diameter, chips pack in the flutes and coolant has trouble reaching the tip. When packed chips grip the drill, the torque rises sharply and the drill breaks.
Peck drilling drills a little, pulls out of the hole to clear the chips and goes back in, repeating the sequence. G83 is the canned cycle that handles this repetition in one block.
Block structure
| Address | Meaning | Example value |
|---|---|---|
X Y | Hole position | X10 Y10, X30, X50 |
Z | Hole bottom depth | Z-25 |
R | R point: the height where rapid changes to cutting feed | R3 (3 mm above the top of the workpiece) |
Q | Depth of each peck (incremental, always positive) | Q5 |
F | Cutting feed | F120 mm/min |
G98/G99 | Height to return to after each hole | See the explanation below |
The sequence for drilling one hole
- Rapid down from the current height (the initial point, Z30 in the example) to the R point Z3.
- Feed in by Q (5 mm) at cutting feed.
- Retract fully at rapid to the R point to clear the chips.
- Rapid back down to slightly above the previous depth (a clearance d set by a controller parameter).
- Cut another Q. Repeat steps 3–5 until the bottom Z-25 is reached.
- Return to the initial point with G98, or to the R point with G99.
Three-hole example
Canned cycles are modal, so after one G83, writing just the coordinates keeps drilling holes under the same conditions. In the drawing, the sawtooth up-and-down motion at each hole is the pecking, and you can see the tool rise high only after the last hole.
Three 25 mm deep holes drilled with Q5 pecks, returning to the initial point only after the last hole
O2007
T5 M6
G21 G90 G17 G94
G54
S1200 M03
G00 X10. Y10. Z30.
G43 H5 Z30.
G99 G83 X10. Y10. Z-25. R3. Q5. F120
X30.
G98 X50.
G80
G00 Z100.
M30The figure above is the CNC Path Analyzer result for this program (rapid 40 segments, linear cutting 18 segments).
How to choose between G98 and G99
G99 (return to R point) shortens the travel between holes and reduces cycle time. Use it when there are no obstacles such as clamps, steps or bosses between holes. G98 (return to initial point) goes back up to the height at which the cycle started, so it is safe when a tall obstacle lies on the way to the next hole.
The example drills the first two holes quickly with G99 and switches to G98 at the last hole, rising to the initial point Z30 before ending the cycle. In practice, G98/G99 are often mixed hole by hole depending on the hole layout and fixture shape.
The difference from G73
G73 is high-speed peck drilling: instead of retracting to the R point each time, it backs off only a short distance to break the chip. The short travel makes it fast, but the chips do not fully leave the hole. G73 is the default choice for relatively shallow holes in materials whose chips break easily, and G83 for deep holes or materials that form long chips.
Drill point angle and estimating cycle time
Z-25. is the depth of the drill tip. A standard drill has a 118° point, so if you want the full diameter to reach 25 mm, you must go deeper by the length of the point. The point length is roughly diameter × 0.3, so for a Ø8 drill you add about 2.4 mm and command around Z-27.4. This is especially important when securing tapping depth in blind holes.
Cycle time can also be estimated. Cutting the 28 mm from R3 to Z-25 at F120 takes 14 seconds of pure cutting. With Q5, the tool retracts to the R point and comes back five or six times per hole, adding rapid round trips that get longer as the hole deepens. Three holes take about 42 seconds of cutting alone, so if chip evacuation is not a problem, there is room to save time just by increasing Q or switching to G73.
Caution when you see G83 on a lathe
On a lathe, G83 (face drilling) may not use addresses the same way as on a machining center. In some formats of the FANUC lathe family, R is interpreted as the incremental distance from the initial point to the R point, and Q may not accept a decimal point. The same text can mean a completely different depth depending on the machine type and controller series.
Because of this difference, CNC Path Analyzer does not invent a path when the meaning of R in lathe G83 is not established, and instead guides the user to confirm the interpretation. The related behavior is covered in Path troubleshooting.
Frequently asked questions
What happens if I forget G80?
G80 when it is finished.