Canned Cycles: Drilling, Boring, Tapping, and Pocketing

What Is a Canned Cycle?

A canned cycle is a pre-programmed, single-block shortcut that tells the CNC control to perform a fixed sequence of moves — rapid down to the R-plane, feed into the workpiece, and return — without you writing every motion line by line. On a Haas mill, canned cycles live in the G80–G89 range. Once a canned cycle is active, it repeats at every XY position you list until you cancel it with G80. This saves dozens of lines of code and eliminates transcription errors on multi-hole patterns.

The R-Plane and Z-Depth

Every canned cycle uses two critical depth parameters:

• R (Reference plane): The Z height where the spindle switches from rapid to feed. Set R high enough to clear all clamps and workpiece features — typically 0.100 in. above the part surface when no obstacles are present.
• Z (Final depth): The bottom of the hole. Always calculate from the same datum (usually the top of the part when using G54 work offset). A Z value that is not deep enough leaves a partial hole; one that is too deep can break a tap or crash a boring bar.

Both R and Z are modal: they stay active at every subsequent XY position until you change them or cancel with G80.

Common Canned Cycles

G81 — Standard Drill

Feed straight to Z-depth, then rapid out. Use for short holes where chip evacuation is not a concern.

```

G81 X__ Y__ Z__ R__ F__

```

G83 — Peck Drill (Full Retract)

Drills in increments (pecks), fully retracts to the R-plane between each peck to clear chips, then rapids back to just above the previous depth before feeding again. The peck increment is set with Q (always a positive value in inches). Use G83 for holes deeper than approximately three times the drill diameter, for difficult-to-machine alloys, or whenever chip packing is a risk.

```

G83 X__ Y__ Z__ R__ Q__ F__

```

G84 — Right-Hand Tapping

Feeds to Z-depth at the calculated pitch feed rate, then reverses spindle direction and feeds back out. The feed rate must equal spindle RPM × pitch (inches per revolution). Getting this wrong strips threads or breaks taps — double-check every time.

```

G84 X__ Y__ Z__ R__ F__

```

G85 — Boring (Feed In, Feed Out)

Feeds to Z-depth, then feeds back out. The feed-out prevents the boring bar from dragging a witness mark on retract. Use for finish-bored holes where surface finish matters.

```

G85 X__ Y__ Z__ R__ F__

```

The L Word

L specifies the number of times a canned cycle repeats at the same XY position (or used with incremental positioning to step through a pattern). L1 is default. L0 loads the cycle parameters without executing — useful for setting up before the first hole position.

Bolt-Circle Patterns

A bolt circle is a set of holes evenly spaced around a center point at a fixed radius. To find each hole's XY coordinates, use:

• X = BC_center_X + Radius × cos(angle)
• Y = BC_center_Y + Radius × sin(angle)

For 6 holes equally spaced, the angles are 0°, 60°, 120°, 180°, 240°, and 300°. Calculate all six positions before you write a single line of G-code and record them on your worksheet — errors here cause scrap.

Tapping Feed Rate

For G84, the feed rate in inches per minute is:

F = RPM × (1 ÷ TPI)

where TPI is threads per inch. For example, a ¼-20 tap at 300 RPM needs F = 300 × (1/20) = 15.0 in./min. Using any other feed rate risks a broken tap or stripped thread.

Program Structure for a Canned Cycle Sequence

A safe sequence for a center-drill → peck-drill → tap operation looks like this:

1. Tool change and spindle start (center drill)

2. G81 — spot all hole positions, then G80

3. Tool change and spindle start (tap drill)

4. G83 with Q peck increment — drill all positions, then G80

5. Tool change and spindle start (tap)

6. G84 with calculated F — tap all positions, then G80

7. G28 or G91 G28 Z0 — return to home

Always verify R-plane clearance after every tool change; a longer tool can crash into a clamp that a shorter center drill cleared.

Safety Points

• Never reach into the machine envelope while a canned cycle is running. Pecking cycles move fast between pecks; a hand near the spindle can be struck.
• Verify your simulation shows no collision alarms before running on the machine.
• Confirm the workpiece is fully clamped and the vise handle is removed before cycle start.
• Coolant nozzles must be aimed before starting; re-aiming with the spindle turning is a laceration hazard.
• When tapping, verify spindle orientation and M29 rigid tapping mode if your control requires it — consult the machine manual.
• Apply lockout/tagout (LOTO) any time you reach inside the machine to set up, adjust clamps, or clear chips. Pressing E-stop alone is not LOTO.