CNC Machinist Calculator UltraHome › G-codes › Haas NGC › G73
G73 High speed peck drilling cycle / Irregular path stock removal cycle
Haas NGC G-code · Mill, Lathe
On mills: High speed peck drilling cycle
Peck drills with a short retract after each peck to break the chip, without leaving the hole. Faster than G83 for shallow to medium holes.
Format
Addresses
| Address | What it does |
|---|---|
X Y | Hole position |
Z | Hole bottom |
R | R plane |
Q | Constant peck depth |
I | First peck depth when Q is not used |
J | Amount each peck is reduced |
K | Smallest peck depth |
P | Dwell at the bottom |
F | Feed rate |
L | Number of holes for repeats in G91 |
How it works
Modal, canned cycle group 09. Cancel with G80.
Example program
G90 G54 G00 X1. Y1. S3000 M03 (FIRST HOLE)
G43 H04 Z1. M08 (APPROACH)
G73 G99 Z-.75 R.1 Q.1 F12. (PECK .1 PER PASS)
…
The full 6-line example is in the app. Example is in inch. Check offsets and clearances first.
Watch out for
- The retract distance after each peck comes from Setting 22.
- Chips stay in the hole. Use G83 for deep holes to clear chips.
On lathes: Irregular path stock removal cycle
Roughs by repeating the finish path offset outward, D times. Made for castings and forgings that already have the rough shape.
Format
Addresses
| Address | What it does |
|---|---|
P | Block number where the path starts |
Q | Block number where the path ends |
D | Number of roughing passes |
I | X distance from first cut to last, radius |
K | Z distance from first cut to last |
U | X finish allowance, diameter |
W | Z finish allowance |
F | Roughing feed rate |
S | Spindle speed |
T | Tool and offset |
How it works
Non-modal, group 00. G18 must be active.
Example program
G96 S400 M03 (CSS 400 SFM)
G00 G54 X2.5 Z.25 M08 (START POINT)
G73 P10 Q20 I.15 K.05 D3 U.02 W.005 F.01 (3 PASSES ON CASTING)
…
The full 8-line example is in the app. Example is in inch. Check offsets and clearances first.
Watch out for
- On bar stock G73 cuts a lot of air. Use G71 or G72 for bar.
- I and K are the total stock to remove, not the depth per pass.
- Only F, S and T before or on the G73 block are used while roughing.
Related codes
G83 · G80 · G98 · G99 · G70 · G71
G73 on other controls
The same number can mean something different on another control.
| Control | Meaning |
|---|---|
| Fanuc | High speed peck drilling |
| Mazak (EIA) | High speed peck drilling |
| Okuma OSP | High speed deep hole drilling |
| Mitsubishi M70 M80 | High speed peck drilling |
| Brother Speedio | High speed peck drilling |
| Heidenhain TNC (ISO) | Rotation of the coordinate system |
| Fagor 8055 8065 | Pattern rotation |
| LinuxCNC Tormach | Chip breaking drill cycle |
| Mach3 Mach4 | High speed peck drill |
| Centroid CNC12 Acorn | High speed peck drilling cycle |
| Hurco WinMax (NC) | High speed peck drilling |
| Fadal | Peck drill, chip break |
| Swiss (Citizen Star) | Pattern repeat cycle |
Every G-code for Haas NGC in your pocket. The app has the full example programs, search by number or shop word, a line decoder and calculators for tapping, threading and drilling.
Open G73 in the app All Haas NGC G-codes