Hello everyone.
I have a question about codes G10/G11 (Fanuc 31i). I know, G10 is used to transfer data into the system via program. I want to use the code G10 for automatic adjustment of the coordinate system (G10 L2 P1 X_Y_Z_). Do I need to use the code G11? When i need used this code? I do not have info in guide, except that this option. Code G10 works on my machine.
The only time I have ever used a G11 is when changing parameters or tool life management. Neither I want left open for accidental adjustments by a program or operators.
As for tool or work offsets I just command the G10 and go, never added a G11 for this.
Yes.
A difference from other applications of G10 is that it behaves as a modal code, when used for parameter entry. Once it enters parameter entry mode, as many parameters as desired can be entered in subsequent blocks, till this mode is cancelled by G11.
In other applications, G10 remains effective only in the block where it is commanded, like a non-modal code. In the next block, if G10 is needed again, it has to be explicitly commanded. Obviously, there is no need to program G11 in such cases.
Thanks for the replies. If anyone has the instructions for use the code G10/G11, please share
Hi
I don't write in Russian, as it's English language forum.
I can send you russian manual for 0i series. there is info about using G10 in it
report me your email
nothing to say under this line
This macro uses G10/G11 to set the X/Z 2nd Zero position. The operator moves X and Z to where he wants the G30P2 (2nd Zero) and runs the macro.Originally Posted by alexium2007
%
O9010 (G30 AUTO-SET)
#101=#5021*25400.
#102=#5022*25400.
G10L50 (PROGRAMMABLE PARAMETER INPUT MODE)
N1241P1R#101 (SET 1241 X TO CURRENT X MACHINE POSITION)
N1241P2R#102 (SET 1241 Z TO CURRENT Z MACHINE POSITION)
G11 (CANCE G10 MODE)
M30
%
dcoupar, Thanks for the example. Now I understand how it works G10/G11.
guhl, I sent the email to you in a personal. Thank you
Posting Permissions
LinkBack URL
About LinkBacks
