y move triggers x over travel range

[rxdeath]

anyone know why a g28 y0.  would cause an x over travel alarm???

it's not work offset, no chips in the machine, other easy stuff, etc

its the last line of a subroutine and put in a g28 y0 after the g91 g28 z0  because i want it to home in z and then bring the part forward.  upon reading i know i can do this wit ha g28 g91 x0 y0 z6.0 or something of the sort to set an intermediate position, but this isn't' the question.

 

it does the  g91 g28 z0. no problem, then alarms out on next line, g28 y0.  with a 1.316 x over travel range alarm...wtf

more important than figuring out a way around it (which i've already done)  WHY does this happen?  what do i not get that could cause a y move to over travel in x?

[Greg Williams]

Can you use G53?

[Leon82]

Is the control reading ahead? Sometimes it will stop before the line has been executed.

 

Also your y move may put the machine in a programed saftey zone. Our yasda is like that. There is a 3d area it won't travel to because of the tool change setup.

[crazy^millman]

What kind of machine is it? Certain machines have certain methods in which you must do things. Like mentioned by Leon give better details and we might be able to assist. 

[Colin Gilchrist]

Do you possibly have TWP (G68.2) active? Just check to see if you might need a G69 before the G28?

I have never been a fan of G28 and G91. It's just too easy to get errors with the combination of Machine Parameters that can be configured to cause a crash or over travel situation.

I always choose to output G53 moves for any safe retract or machine positioning move. The main reason I love G53 is that it won't cancel your active work offset, and when G53 is read, the machine temporarily disables look ahead. The final reason is that I can make all the safe moves using Absolute Coordinates (G90), so I never have to worry about where I reset the machine in the NC Program, because my code never puts the machine in Incremental Mode for a repositioning or safe retract move.

[So not a Guru]

3 minutes ago, Colin Gilchrist said:

I always choose to output G53 moves for any safe retract or machine positioning move.

This won't work on many routers, as the G53 Z position is the bed of the machine. Don't ask me how I know this

Does the line have G91 G28 Y0 , or is it just G28 Y0 without the G91 call?

[rxdeath]

it is a haas vf1

this is the last few lines of the program

g91 g28 z0.

g28 z0.

g90

m99

 

colin, as i was typing my responses i realized you probably nailed it.  i do have g68 active  at a very slight angle < .1 degrees usually.  but that would likely do it over the course of the whole table moving back.  well played, sir thank you