How do I cancel look ahead on Haas

[Bob W.]

Anyone know which G-code cancels look ahead on a Haas? Also, on the Fanuc control G53 acts as a barrier that the look ahead can't see past. Does Haas have a similar code, or does G53 on a Haas function in the same manner?

 

Lastly, once look ahead is canceled how do I activate it again? I disable/ enable look ahead for some macro logic to compute correctly.

[Allan]

G130 P0 will cancel the look ahead. (the P controls how many blocks to look ahead up to 15)

EDIT S/B G103 P1 one block look ahead....

G187 will turn it back on.

EDIT G103 P0 would turn it back on....

 

 

G53 is a one shot call to machine co-ordinates on a FANUC and a HAAS, not suppose to turn off Look ahead AFAIK, could be a side affect.

 

 

Allan

Edited March 20, 2014 by Allan

[GoetzInd]

Bob,

Pretty sure there is a setting to turn off the option. Also, are you using G187 Px? What are you trying to accomplish by turning off look ahead?

 

Mike

[Bob W.]

I don't want the look ahead causing issues when setting values for macro calculations. I want to turn it off, do all the calculations, then turn it back on.

[Robert Ouellette]

you are looking for G103. type in G103 p1 and you get 1 line of code look ahead. t cancel type in g103 p0. sets it to unlimited.

[Colin Gilchrist]

Robert is correct. G103 P1, followed by G103 or G103 P0. You also must cancel cutter compensation before commanding G103. G103 P[xx], where P is 1-15, specifying the number of blocks to look ahead.

 

There are also 3 settings that affect Macro programs:

There are 3 settings that can affect macro programs (9000 series programs),

these are 9xxxx progs Lock (#23), 9xxx Progs Trace (#74) and 9xxx Progs

Single BLK (#75).

[Bob W.]

My concern is specifically related to M98 program calls. In the past on my VM3 I have had a master program that called subs like this:

 

M98 P1

M0

M98 P2

M0

M98 P3

M0

M99

 

The control called the wrong sub and the only thing we could think of was that it was related to look ahead. We are currently running parts that would really benefit from this but I want to make sure it runs correctly.

[Newbeeee™]

Bob,

Regarding Fanuc and especially 31i control, I remember being told something similar regarding macro's being skipped as the control read 'too fast'.

Again by memory, a dwell (G04X#) had to be programmed to momentarilly stop the control from continuing past what wanted to be read.

Foghorn may be able to clarify this?

[Tim Johnson]

Bob,

Regarding Fanuc and especially 31i control, I remember being told something similar regarding macro's being skipped as the control read 'too fast'.

Again by memory, a dwell (G04X#) had to be programmed to momentarilly stop the control from continuing past what wanted to be read.

Foghorn may be able to clarify this?

 

Adding a block number by itself on a line will stop "fast processing" till the empty block is read. (on Fanuc)

[Machineguy]

Do it like Robert said in post #5.

g103 p1 before the macro

g130 p1 after.

 

Machineguy

[Robert Ouellette]

I need to do that when ever I put probing routine in my programs. the probing sub programs call up g103 p1 to cancel read ahead and when you run your program without canceling it they error out and will not run properly. so I put the g103 p0 after I call my probing and all runs fine.