G81, G82, G83 and G73: Drilling Canned Cycles

A canned cycle packs the moves for drilling a hole into one line. Instead of writing a rapid to the hole, a rapid down, a feed to depth and a retract, you give the cycle a position, a depth and a feed rate, and the control does the rest.

The common drilling cycles all use the same words:

After each hole, the tool returns either to the R plane or to its starting height. That is set by G98 and G99.

The cycles

• G81: drilling. Feed to Z, rapid out. Use it for spot drilling and shallow holes.
• G82: drilling with a dwell. Like G81, but the tool pauses at the bottom for the P time. The dwell cleans up the bottom of spot-drilled, countersunk or counterbored holes.
• G83: peck drilling. Feeds down by Q, rapids back out to the R plane to clear the chips, then rapids back down to just above the last depth and feeds the next peck. Use it for deep holes.
• G73: high-speed peck drilling. Pecks by Q like G83, but backs off only a short distance to break the chip instead of leaving the hole. Faster than G83, but chips stay in the hole.
• G85: boring. Feeds in and feeds back out, for reamed or bored holes where a rapid retract could mark the wall.
• G80: cancel. Ends the cycle.

Other cycles cover tapping (G84) and other boring operations (G86, G88, G89).

Canned cycles are modal

Once a cycle starts, every following line with an X or Y position drills another hole using the same Z, R, F and Q, until G80 or another motion code such as G00 or G01 cancels it. That's why drilling a row of holes only needs the new position on each line:

G81 X10 Y10 Z-5 R2 F150
X30
X50
G80

Example: drilling, dwelling and peck drilling

This program drills two plain holes with G81, a third with a dwell using G82, and a 20 mm deep hole with G83. G99 keeps the tool at R2 between the first three holes, and G98 sends it back to Z25 after the deep hole.

(Drilling cycles example: G81, G82 and G83 in one program)
G21 G17 G90 G54
T1 M6 (6 mm drill)
S1800 M3
G0 X10 Y10 Z25
(G81: plain drilling, 5 mm deep, return to R2 between holes)
G99 G81 X10 Y10 Z-5 R2 F150
X30
(G82: the same hole with a 0.5 second dwell at the bottom)
G82 X50 Y10 Z-5 R2 P500 F150
(G83: peck drilling 20 mm deep, 4 mm per peck, then back to Z25)
G98 G83 X30 Y35 Z-20 R2 Q4 F120
G80
G0 Z25
M5
M30

• G99 G81 X10 Y10 Z-5 R2 F150 rapids to X10 Y10, rapids down to R2, feeds to Z-5 at 150 mm/min and rapids back to R2.
• X30 drills the second hole with the same cycle.
• G82 ... P500 changes to G82 and dwells for 500 ms at the bottom. On Fanuc and Haas, P without a decimal point is in milliseconds; on LinuxCNC it would be seconds.
• G98 G83 ... Z-20 R2 Q4 peck drills 20 mm deep in 4 mm pecks, and returns to Z25 afterwards.
• G80 cancels the cycle before the final G0 Z25.

Machine differences

• GRBL doesn't support canned cycles, so CAM software writes the hole moves out in full.
• Mach3, LinuxCNC, Fanuc and Haas support G73 and G81–G89.
• The small retract in G73 is set by a machine parameter on Fanuc-style controls, not by the program.

How CutViewer shows drilling cycles

CutViewer draws each hole in a G73, G74 or G81–G89 cycle as a rapid to the hole position, a rapid down to the R plane, a feed to the hole depth and a retract, using G98 or G99 for the retract height. G85 and G89 (and the tapping cycles G74 and G84) feed back out; the others rapid out. Pecks (Q) and dwells (P) are not drawn separately, so a G83 hole looks like one feed to full depth. Repeat counts (K or L) drill the hole that many times, and in incremental mode (G91) each repeat steps by the X and Y on the line, with R measured from the initial Z and Z from the R plane. L0 or K0 stores the cycle without drilling. G80 or any motion code ends the cycle.