Haas Mill · G-code
G10 Set Offsets from the Program
Writes work offsets, tool lengths or diameters into the offset tables directly from a program line.
What G10 does on a Haas mill
G10 lets the program load values into the control's offset pages, so a setup can be repeated without anyone typing numbers by hand. The L address selects which table, P selects which entry.
Common Haas uses are L2 for G54–G59 (P1 = G54 … P6 = G59), L20 for the extended G154 offsets, and L1/L10 to L13 for tool length and diameter geometry and wear. G90 writes the value, G91 adds to it.
G10 format
| Address | Meaning |
|---|---|
L2 P1–P6 | Work offsets G54–G59 |
L20 P1–P99 | Extended offsets G154 P1–P99 |
L1 / L10 | Tool length geometry |
L11 | Tool length wear |
L12 / L13 | Tool diameter geometry / wear |
X Y Z R | Values to write |
G10 example program
G90 G10 L2 P1 X-10.2516 Y-6.0381 Z0. (load G54)
G91 G10 L11 P5 Z-0.002 (add -0.002 to T5 length wear)
G90⚠ Watch out
G10 in G91 adds to whatever is already there. Running the same block twice doubles the change. Put G90 on the very next line so the rest of your program is not left in incremental.
Related codes
G10 questions
How do I set G54 from a program on a Haas?
Use G90 G10 L2 P1 followed by the X, Y and Z values. P2 is G55, up to P6 for G59.
Independent reference. Not affiliated with, sponsored by or endorsed by Haas Automation, Inc. Haas is a trademark of its respective owner. Always confirm codes against your machine's operator manual — options and settings vary by model and software version.