[DingoHammer]

I have a 2005 Haas tool room mill. G52 X1.0 is ignored. Also, G10 L2 P0 G90 X1.0 is ignored. I can, however, manually enter values for G52 in the offsets page.

According to the manual both of these commands should work. I have tried both the Fanuc and Haas options for G52. Is there a setting somewhere that disables G52? Is G52 capability an option that has to be purchased?

Thanks
DH

[Matt@RFR]

Out of curiosity, what does this do on your mill?

#5201=1.

That should do exactly the same thing as entering G52 X1.

[Geof]

G52 is a standard G code on Haas machines not an option.

Can you post an example of a program written with G52 commands that will not work on your machine?

What is Setting 33 set at, Fanuc, Yasnac or Haas? Yasnac treats G52 in a different manner to the other two.

[DingoHammer]

The problem seems to have resolved itself. I tested an example program to post here and it worked. I tested the program that had been giving me problems and now it works. Maybe turning the machine off for a couple of days reset something that was causing the problem.

Thanks for the replies.

DH

[DingoHammer]

The problem is solved. Setting 31 is the option for how G52 is interpreted. in the default Yasnac mode, G52 is treated the same as a G54, G55, etc. offset and a command such as G52 X1. issued within a program has no effect. In Fanuc mode, G52 it is treated as a work shift and a G52 X1. will shift the X origin 1 inch until it is cancelled by another G52 command.

When changing setting 31, power cycle the machine to make sure the setting takes effect.

[haastec]

When changing setting 31, power cycle the machine to make sure the setting takes effect.

You should not have to cycle power.
With all settings, change to the desired action and press the ENTER button. Many people forget to press enter which will change the setting back to the previous state when exiting the settings page.

[Geof]

Actually it is Setting 33 not Setting 31. Which is why I asked about Setting 33.