Question on using g10 for work offsets HMC Fanuc

[Shotout]

I have not been able to find this in the manuals for the Fanuc control (310is). We use G10 to set the work offsets, normally center or rotation of the rotary axis, but I haven't been able to find out what the L address signifies. Our programs that predate me use L2 but I'd like to understand why and how it is used. I'd appreciate any illumination that someone is willing to share.

Thanks
Scott

[dcoupar]

L2 specifies the standard WCS (1 to 6 - G54 to G59) (see attached .jpg)
L20 specifies the additional WCS (1 to 48 - G54.1 P1 to P48)
Also remember, G91 can be used to add or subtract from the value currently in the register.

So:

G10 L2 P2 X-12.3456 sets X of G55 to -12.3456

G10 L20 P2 X-12.3456 sets X or G54.1 P2 to -12.3456

G91 L20 P6 X-0.03 reduces the value in G54.1 P6 by 0.03.

[Shotout]

So the only values for L are 2 which sets G54-G59 depending on the P value of 1-6, or 20 which allows for 48 additional WCS that would be called in a program as G54.1 Pnn. Is that correct?

Originally Posted by dcoupar L2 specifies the standard WCS (1 to 6 - G54 to G59) (see attached .jpg) L20 specifies the additional WCS (1 to 48 - G54.1 P1 to P48) Also remember, G91 can be used to add or subtract from the value currently in the register. So: G10 L2 P2 X-12.3456 sets X of G55 to -12.3456 G10 L20 P2 X-12.3456 sets X or G54.1 P2 to -12.3456 G91 L20 P6 X-0.03 reduces the value in G54.1 P6 by 0.03.

[beege]

No, L2 and L20 have to do with the work offsets, but other "L"s are for things like parameters, tool offsets, pitch comp, and things you usually don't want to mess with from inside a program.

[Shotout]

Originally Posted by beege No, L2 and L20 have to do with the work offsets, but other "L"s are for things like parameters, tool offsets, pitch comp, and things you usually don't want to mess with from inside a program.

OK. I appreciate the explanations thanks.