Drill Calculator logoDrill Calculator
ISO / Fanuc / Haas G-Code Programming

CNC-Bohrzyklen (G81, G82, G83, G73)

Canned cycles condense complex multiaxis peck drilling and retract sequences into a single modal G-code block. Understanding the mechanics of retraction planes (G98/G99) and chip evacuation cycles prevents tool breakage and workpiece collision.

G81: Straight Drilling

No Dwell / No Peck

Feeds continuously from reference plane R to final depth Z at programmed feed rate F, then rapids straight back out. Ideal for shallow holes (< 3× diameter) and spotting.

G98 G81 Z-15.0 R2.0 F200

G82: Counterbore with Dwell

Bottom Dwell (P)

Feeds continuously like G81, but pauses (dwells) at hole bottom for P milliseconds (or seconds) before retracting. Cleans up bottom face finish and eliminates cutter bounce.

G98 G82 Z-6.0 R2.0 P500 F150

G83: Deep Hole Full Retract Peck

Full Clearance (Q)

Drills incrementally by peck depth Q, then completely rapids back out to the R plane to evacuate chips and flood flutes with coolant. Essential for deep holes (> 3–5× diameter).

G98 G83 Z-40.0 R2.0 Q4.0 F220

G73: High-Speed Chip Break Peck

Fast Relief (0.5mm)

Drills by Q depth, then backs up only 0.5 – 1.0 mm to snap the chip string before immediately resuming feed. Greatly reduces cycle time when deep clearance isn't required.

G98 G73 Z-25.0 R2.0 Q3.0 F250

Return Plane Mechanics: G98 vs G99

Every canned cycle requires choosing between two modal return planes:

G98: Return to Initial Plane

After completing the hole, the spindle rapids all the way back up to the Z height it occupied before the canned cycle was called.

✓ Mandatory when jumping over toe clamps or vice jaws.
G99: Return to R Reference Plane

The spindle retracts only to the programmed R plane (usually 1.0 - 2.5 mm above the part face) before moving to the next X/Y coordinate.

✓ Maximum cycle time efficiency across flat, unobstructed surfaces.

Crucial Safety Rules for Canned Cycles

  • Always Cancel with G80: Canned cycles are modal. If you move X/Y on the next line without commanding G80, the machine will drill another hole at that location!
  • Always Specify Decimal Points: In Fanuc controls, Q2 without a decimal point is interpreted as 0.0002", causing endless micro-pecks. Always program Q2.0.
  • R-Plane Below Surface Danger: Ensure your R plane is positive relative to the part Z0. Setting R below the workpiece face causes the drill to rapid directly into solid metal.

Interactive CNC Canned Cycle Generator

Generate ready-to-run Fanuc & Haas G-code with PCD bolt hole circles, coordinate arrays, and automatic peck schedules.

G-Code Generator →Peck Depth Tool