CNC Machinist Calculator UltraG76 Fine boring cycle / Multiple pass threading cycle
Fanuc G-code · Mill, Lathe
On mills: Fine boring cycle
Bores to depth, stops the spindle in an oriented position, shifts the tool off the wall by Q and rapids out so the bore is not scratched.
Format
Addresses
| Address | What it does |
|---|---|
X Y | Hole position |
Z | Hole bottom |
R | R plane where feed starts |
Q | Shift amount at the bottom, always positive |
P | Dwell at bottom, milliseconds |
F | Feed rate |
K | Number of repeats |
How it works
Modal, group 09. Cancel with G80 or any group 01 code.
Example program
G90 G54 G00 X2. Y1.5 S1200 M03 (BORE CENTER)
G43 H08 Z1. M08 (CLEARANCE)
G98 G76 Z-1. R.1 Q.005 F4. (FINE BORE, SHIFT .005)
…
The full 5-line example is in the app. Example is in inch. Check offsets and clearances first.
Watch out for
- The shift direction is set by a parameter. Set the boring bar tip to point the opposite way, or it digs into the wall.
- Q must be positive. A minus sign is ignored and the parameter direction is used.
- Keep Q small, a few thousandths. A large shift can hit the wall on small bores.
On lathes: Multiple pass threading cycle
Cuts a full thread from two lines with infeed along one flank, a falling depth per pass and spring passes. P on the first line packs finish passes, chamfer and tool angle into six digits.
Format
Addresses
| Address | What it does |
|---|---|
P (first block) | Six digits: m finish passes, r end chamfer in tenths of lead, a tool angle |
Q (first block) | Minimum depth of cut, radius value, no decimal point |
R (first block) | Finish allowance |
X Z | Thread minor diameter and thread end |
R (second block) | Taper, radius difference from start to end, 0 for straight |
P (second block) | Thread height, radius value, no decimal point |
Q (second block) | First pass depth, radius value, no decimal point |
F | Lead, 1 divided by threads per inch |
How it works
Non-modal.
Example program
G97 S800 M03 (CONSTANT RPM)
G00 X.85 Z.3 M08 (START 3 LEADS BEFORE)
G76 P020060 Q20 R.001 (2 SPRING PASSES, NO CHAMFER, 60 DEG)
…
The full 6-line example is in the app. Example is in inch. Check offsets and clearances first.
Watch out for
- P and Q values take no decimal point. In inch, P613 is .0613 thread height.
- Start the tool at least 3 leads before the thread so the axis is up to speed.
- Use G97 constant RPM, never G96.
Related codes
G85 · G86 · G87 · G80 · G98 · G99 · G92 · G32 · G97
G76 on other controls
The same number can mean something different on another control.
| Control | Meaning |
|---|---|
| Haas NGC | Fine boring cycle |
| Mazak (EIA) | Fine boring cycle |
| Okuma OSP | Fine boring cycle |
| Mitsubishi M70 M80 | Fine boring cycle |
| Brother Speedio | Fine boring cycle |
| Fagor 8055 8065 | Probing move while touching |
| LinuxCNC Tormach | Lathe multi pass threading |
| Mach3 Mach4 | Fine boring, Mach4 |
| Centroid CNC12 Acorn | Fine boring cycle |
| Hurco WinMax (NC) | Fine boring with orient |
| Fadal | Fine boring with oriented shift |
| Swiss (Citizen Star) | Multiple pass threading cycle |
Every G-code for Fanuc 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 G76 in the app All Fanuc G-codes