Common to all Haas control systems is the standard G10 function – a feature optional at extra cost on other controls. The G10 code has a variety of uses, not least being the ability to programmable move offsets and also set offsets from within the program – what are the benefits of this?
Firstly, the operator/setter does not need to ensure the correct offsets are stored with the right program as the data is within the program itself, therefore only the program is stored.
Secondly, since offsets can be moved using this feature within the program itself, sub-routines are simplified through the use of a common offset which is moved accordingly.
The format is laid out below:
G10 allows the programmer to set offsets within the program. Using G10 replaces the manual entry of offsets (i.e. Tool length and diameter, and work coordinate offsets).
L – Selects offset category where;
P – Selects a specific offset where:
R Offset value or increment for length and diameter.
G10 L2 P1 G91 X60. ——- Moves offset G54 X-axis 60 mm to the right
G10 L20 P2 G90 X100. Y80. ——- Sets offset G111 to X100. Y80. from the home position
G10 L10 G90 P5 R250. ——- Set tool length offset for tool 5 to 250mm
G10 L12 G90 P5 R28. ——- Set tool diameter offset for tool 5 to 28mm
G10 L20 P50 G90 X100. Y250. ——- Set work offset G154 P50 to X100. Y250.