What Is a Canned Cycle in CNC Machine Control?

• 1
  How a canned cycle in a CNC machine actually runs
• 2
  Which G-code belongs to which operation
• 3
  Where canned cycles stop being the right answer
• 4
  What we check before a cycle goes into production
• 5
  Writing and proving a drill cycle in five steps
• 6
  Cycle selection by feature, not by habit
• 7
  Canned cycle or CAM toolpath: quick decision table

A canned cycle is a fixed motion sequence burned into the control. Instead of writing out every rapid, feed, retract, and return move for each hole, the programmer writes one G-code line that starts the cycle and then lists positions. The control expands each position into the full motion internally.

The word canned is old shop slang for pre-packaged. On a Fanuc-style control the cycle lives in firmware, so the same G81 behaves the same way on a lathe control, a mill, and a machining center of the same family. That predictability is the point.

Four values drive every drilling-family cycle. X and Y are hole center coordinates. Z is the final depth, measured to the tip of the tool, not the shoulder. R is the retract plane where the tool switches from rapid to feed. Q, where the cycle needs it, is the peck depth or shift distance.

One detail trips up new programmers. Z depth is not the depth of the hole. It is the final Z position of the tool tip. If you want a Ø 8 mm drill to break through a 10 mm plate, Z must be programmed past the bottom face by roughly a third of the drill point length, or the hole will not be round at the exit.

• 1
  Modal behaviorThe cycle stays active until G80 cancels it or another cycle replaces it.
• 2
  Initial planeThe Z value before G81 is the clearance plane the tool returns to.
• 3
  R planeSet it 1–3 mm above the stock so chips clear before the feed starts.
• 4
  Single-shot modeG98 returns to the initial plane between holes; G99 returns to R.

G81 is the plain drill cycle. The tool feeds to Z, then rapids out. It suits shallow holes up to about three times the drill diameter, where chip evacuation is not a problem and the drill does not wander.

G83 is the deep-hole peck cycle. The tool feeds by Q, retracts fully to R, then feeds again from the previous depth. Full retract clears chips out of the flutes, which matters once depth passes three to four times diameter in aluminium and sooner in stainless.

G73 is a high-speed peck that retracts only a small amount instead of going all the way to R. It is faster on ductile materials where chips break cleanly, and a poor choice in gummy materials where chips weld to the flutes.

G82 adds a dwell at the bottom. A 0.2–0.5 s dwell at Z flattens the bottom of a blind hole and improves depth repeatability for counterbores and spotfaces. G85 and G86 cover boring, and G84 turns the same Z motion into a synchronized tap: spindle speed and feed are locked by the thread pitch.

On lathes the same idea appears as G71, G72, G70 for roughing and finishing profiles, G74 and G75 for peck drilling and grooving, and G76 for threading. The structure is identical. One block describes a whole sequence of passes that the control computes from the part profile.

A canned cycle assumes one tool, one spindle axis, and a hole normal to the tool axis. As soon as the surface is angled, curved, or interrupted, the assumption breaks. A hole drilled on a sloped face needs a spot or flat first, or the drill walks and the entry is oval.

On a 5-axis machine, cycles still work on faces that have been indexed normal to the tool. Polar or face-milling cycles on a turned part can drive a live tool through a cross hole accurately, but they cannot compensate for a surface that changes angle during the cut. That is CAM and full interpolation territory.

High-pressure through-spindle coolant changes the economics of pecking. With 70 bar coolant and a proper through-coolant drill, a 5:1 hole may run in one G81 pass with no pecking at all, and cycle time drops sharply. Pulling coolant pressure and peck depth from a generic template is how shops leave money on the table.

The other boundary is machine-specific cycles. Pocket and face cycles from a control builder, such as a rectangular or circular pocket routine, are not portable. A program written with them will not run on a different control family without rewriting, which matters when a job moves between machines or suppliers.

There is a precision limit too. Canned cycles position at the programmed coordinate, and the control handles the motion. Final bore size, roundness, and surface finish still come from tool runout, spindle condition, and the finishing pass, not from the cycle choice.

Depth-to-diameter ratio sets the peck strategy, not the drawing. A Ø 6 mm hole 40 mm deep in 17-4PH stainless behaves nothing like the same ratio in 6061 aluminium. We set Q from chip form, listen to the cut, and adjust.

R plane height is a real cost. Lifting R from 1 mm to 8 mm on a 400-hole pattern adds minutes of air time. We keep R tight, 1–3 mm above the highest point of the stock, and check that the fixture and clamps clear the rapid plane.

Retract mode saves time on large plates. G99 keeps the tool at R between holes, which is what you want when the surface is flat and clear. G98 is safer when clamps, bosses, or step-ups sit between hole positions.

Tool runout decides whether the cycle produces a round hole or an oversized one. A drill with 0.05 mm runout cuts 0.1 mm oversize on a two-flute tool. On bearing seats and dowel holes we pre-drill, then bore or ream, rather than trusting a drill cycle to hold size.

We verify every cycle program on a first article against the drawing, then hold 100% inspection before shipment across the run. Tolerances down to ±0.005 mm (±0.0002 in) and finishes from Ra 0.2–0.8 μm are held with the right tool and pass, not with the cycle alone.

• 1
  Material mattersAluminium breaks chips at high speed; stainless needs shorter pecks.
• 2
  Fixture clearanceCheck clamps against the G98 initial plane, not just the part.
• 3
  Coolant routeThrough-spindle coolant can remove the peck where the drill allows.