What's new
What's new

G54 zeros on reset.

kmuller

Plastic
Joined
Jan 13, 2004
Location
Minden, NV, USA
Fanuc 16i controller. Just got 2 used machines. On one of them, G54 changes to zeros when the reset button is pressed. How can I stop this?
 
reset

Fanuc 16i controller. Just got 2 used machines. On one of them, G54 changes to zeros when the reset button is pressed. How can I stop this?
.
does G55 change on reset? if it does not change use G55 and do not use G54
.
if G55 changes too it has to be a parameter setting
 
The 16i parameter manual is vague when explaining many parameters, so the following parameters I suggest looking at may not be the cause.




parameter 1201 bit 7, WZR: Upon reset, the workpiece coordinate system is:
0 : Not returned to that specified with G54
1 : Returned to that specified with G54



parameter 1202 bit 3, RLC: Local coordinate system is
0 : Not cancelled by reset
1 : Cancelled by reset



There doesn't seem to be any other relevant parameters related to the reset button on the control. I searched a pdf of the 16i manual for the term "reset"

Could possibly be a diagnostic parameter, I suppose, but it would be really weird for the MTB to program it to do that. What make/model machine?
 
Last edited:
Fanuc 16i controller. Just got 2 used machines. On one of them, G54 changes to zeros when the reset button is pressed. How can I stop this?

Are you saying that the values registered for Workshift Offset G54 are set back to Zero when Reset is pressed, or that G54 is cancelled (but values remain registered) when Reset is pressed? If the former, then there is an issue with the control; I'm not aware of any Parameter that can be set to affect the Workshift Offsets in that way. If the latter, then its as dandrummerman21 suggests in Post #3.

Regards,

Bill
 
We have an older Supermax VMC with an O-M control that will zero the G54 when pressing RESET while in "Manual" mode. On our machine there is a toggle button on the control panel labelled MANUAL/ABSOLUTE to turn that "feature" off.
 
we keep G54 on work offset screen all zero
.
we use G55 and higher
.
on a reset if somehow somebody did not notice reset going to zero would be over 70" different. sort of
forces operator to say why is it doing that and to check current modal codes in effect. my Fanuc 15
resets to
G54
G0
G17
G40
G49
G80
H0
D0
G92 is not cancelled which is annoying, requires pressing zero return/home button and cycle start
at zero return spot i check position display and make sure it reads all zeros if G54 is all zeros.
.
basically bad things happen if reset is not noticed
 
Here is how it works on the I series controls:

parameter 1201b7=0 Placed in the reset state (G code is not returned to G54)

parameter 3402b6=0 Cause reset state...1 will cause clear state, which will not put in reset state, which may cause other problems.

parameter 3407b6=1 Does not place G code group (group 14...g54,55,56,etc) in the cleared state.
 








 
Back
Top