G10 Command for G154P1, G154P2 etc...

[ggundrum]

Hi All,

I was wondering if anyone could help me figure out how to use the G10 command to set the coordinates of the G154P1 work coordinate. Specifically what is the P value for these?

[KenFoulks]

Here is an excerpt from the manual, check out the last line:

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.
L2 Work coordinate origin for G52 and G54-G59
L10 Length offset amount (for H code)
L1 or L11 Tool wear offset amount (for H code)
L12 Diameter offset amount (for D code)
L13 Diameter wear offset amount (for D code)
L20 Auxiliary work coordinate origin for G110-G129
P – Selects a specific offset.
P1-P100 Used to reference D or H code offsets (L10-L13)
P0 G52 references work coordinate (L2)
P1-P6 G54-G59 references work coordinates (L2)
P1-P20 G110-G129 references auxiliary coordinates (L20)
P1-P99 G154 P1-P99 reference auxiliary coordinate (L20)
R Offset value or increment for length and diameter.
X Optional X-axis zero location.
Y Optional Y-axis zero location.
Z Optional Z-axis zero location.
A Optional A-axis zero location.

Programming Examples:
G10 L2 P1 G91 X6.0 {Move coordinate G54 6.0 to the right};
G10 L20 P2 G90 X10. Y8. {Set work coordinate G111 to X10.0 ,Y8.0};
G10 L10 G90 P5 R2.5 {Set offset for Tool #5 to 2.5};
G10 L12 G90 P5 R.375 {Set diameter for Tool #5 to .375”};
G10 L20 P50 G90 X10. Y20. {Set work coordinate G154 P50 to X10. Y20.}