CNC Machinist Calculator UltraG50 Scaling cancel / Maximum spindle speed clamp / Coordinate system setting
Fanuc G-code · Mill, Lathe
On mills: Scaling cancel
Cancels scaling started by G51. Positions are no longer multiplied by the scale factor.
Format
How it works
Modal, group 11. Power on default.
Example program
G50 (SCALING OFF)
G00 Z1. (CLEAR)
Example is in inch. Check offsets and clearances first.
Watch out for
- Give G50 in its own block.
- On a Fanuc mill G50 is scaling cancel. On a Fanuc lathe G50 means something else, so do not mix them up.
On lathes: Maximum spindle speed clamp
G50 with an S word sets the top RPM the spindle may reach in constant surface speed mode. Always put it before G96.
Format
Addresses
| Address | What it does |
|---|---|
S | Maximum spindle RPM |
How it works
The clamp stays set until changed. Applies to G96 mode.
Example program
G50 S2500 (CLAMP AT 2500 RPM)
G96 S450 M03 (CSS 450 SFM)
G00 X2.1 Z.1 M08 (APPROACH)
Example is in inch. Check offsets and clearances first.
Watch out for
- Without a clamp, G96 near X0 can run the spindle to its top speed.
- Set the clamp for the chuck, the part grip and balance, not just the tool.
- G50 with X or Z instead resets the coordinate system. Never mix them up.
On lathes: Coordinate system setting
G50 with X and Z tells the control where the tool is right now, which sets the work coordinate system. An older method replaced by G54 and the geometry offsets.
Format
Addresses
| Address | What it does |
|---|---|
X | Current tool position as a diameter in the new system |
Z | Current tool position in Z in the new system |
How it works
Non-modal command. The coordinate system it sets stays.
Example program
G50 X10. Z5. (TOOL TIP IS AT X10. Z5.)
T0101 (FIRST TOOL)
Example is in inch. Check offsets and clearances first.
Watch out for
- If the tool is not exactly where the program expects, every later move is shifted. A crash risk.
- Do not use with G54 style offsets unless the whole program was written that way.
Related codes
G50 on other controls
The same number can mean something different on another control.
| Control | Meaning |
|---|---|
| Haas NGC | Scaling cancel |
| Mazak (EIA) | Scaling cancel, machining center |
| Okuma OSP | Scaling cancel |
| Mitsubishi M70 M80 | Scaling cancel |
| Brother Speedio | Scaling cancel |
| Fagor 8055 8065 | Controlled corner rounding |
| Mach3 Mach4 | Scaling cancel |
| Centroid CNC12 Acorn | Scaling and mirroring off |
| Hurco WinMax (NC) | Scaling cancel |
| Fadal | Ramp slope control cancel |
| Swiss (Citizen Star) | Max spindle speed and coordinate set |
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 G50 in the app All Fanuc G-codes