look ahead parmeter on a fanuc 31i control

[kenfromlodi]

I have a Fanuc 31i control, when I run a macro with a #3006 (program stop with message) the macro program will jump to the end of the program without finishing the remainder of the program. Haas has a similar problem and G103 will control this problem. My question is what parameters in the Fanuc control force the “look ahead off” mode? I have several other 31i controls that work fine, but two of my machines dont and I can not locate the parameters in the Fanuc book. Any fanuc experts out there?? thanks

[Tony35]

you can put some end of blocks in front of the #3006

;

;

;

;

#3006

HTH

[Guest CNC Apps Guy 1]

This on a Toyoda by chance???

[kenfromlodi]

Thanks, We are trying the EOB's now..

 

No, its not a toyoda its a Mori Robo drill

[Guest CNC Apps Guy 1]

You mean FANUC Robodrill???

[Tony35]

i was wondering bout that

[kenfromlodi]

good catch!! we have 22 of them I dont know why I cant get it right.. lol..

[Tony35]

well did it work?

[Guest CNC Apps Guy 1]

There's a G-Code that basically slows the Look-Head function down. Absolutely necessary for running MACRO's. I'm diggin through it now...

[?Mark]

Hey James, check your e-mail.

 

now back to your regular programming...

[Guest CNC Apps Guy 1]

I think I've just put in a 1/2 second dwell before and after. to make sure the calc happens...

[Dave Ball]

James isn't the G code: G08 P0, to turn off look ahead?

[kenfromlodi]

no the EOB's did not do it. We are going to try the dwell. Thanks

[kenfromlodi]

we tried the G08 and it did not work either.

Said it was an invalid code.

[Guest CNC Apps Guy 1]

It is but that's not exactly what's happening... the new controls process so fast that they will often blow by MACRO calcs. Which if you ever goe through a MACRO in single block and it works, yet when you fun at 100% it does not work.. that's often why.

 

Some machines have a M-Code for this type of occurrence and others have a G-Code. I just can;t seem to find it. You may want to hit up Henry, he may know off the top of his head. I do not.

[kenfromlodi]

thanks,

 

the macro works perfectly in single block so we hope that this is the problem. It works great on 20 machines and will not on 2 of them. guess they must be the 2 fastest.. lol

[iowajim62]

quote:

---

You may want to hit up Henry

---

Now your talking, the answer man.

[Guest CNC Apps Guy 1]

Henry is the guy I go to when I'm and I really need a

[Psychomill]

I'd have to check but I think on a 31i its parameter 1604.0 ... This forces default mode of G5.1 which is probably whats blowing by your macros. Someone has a book they can check this one... or even check the state of the machines that work to the ones that don't. I'm not in front of one right now. Like James mentioned, some controls have a G or M code to shut it off but even that might not work because of the parameter state. I just had to switch this on a few new machines which is why the number is sticking in my head I think....

 

Either that or put in a boat load of dwells.. EOBs don't work on fast controls. Funny though... you say "G08" gives you an invalid code alarm? Maybe it wasn't placed correctly?

[yamahaluv]

its the G05.1 Q0 TURNS IT OFF AND GO5.1 Q1 turns it on. If you are running with macro equasions, it will skip all around.

[kenfromlodi]

Actually the G05.1 is giving us alarms also.

Maybe there is another problem since all the other machines are running it fine and these two are not.

I am out of the office today but will give it a shot tomorrow, thanks everyone. I will let you know what happens.

[Guest CNC Apps Guy 1]

If you do not cancel G5.1Q1 with G5.1Q0 AND have a G49 AFTER the G5.1Q0 and before the next G5.1Q1 call, you WILL get alarms. Almost guaranteed.

 

 

1604.0 is correct. That makes AI-NANO on automatically on when the machine is in-cycle. If you run MACRO's this shoudl definitely be OFF. I've always found that it's best to always call it when you want it on. That gives you the most flexibility.

 

 

Just because you have G5.1 Q1 DOES NOT mean you have G8 P1. They are seperate options, besides, comparing G8P1 to G5.1Q1 is like comparing a Ford Pinto to an Accura NSX. Yes there IS that much difference.

 

Technically the "Look Ahead" (G8P1 or G5.1Q1, or G5P10000 for that matter) is not causing the issue. It's the overall speed of the control. Think in terms of a Pentium 3 compared to a high end Xeon server processor. One is going to execute instructions faster than the other. You need to slow that down. I was poring over some MACRO's for a Robodrill this morning for an unrelated matter and found there were numerous G4P1's all over the place where calcs were taking place. For the unitiated that's a dwell for 1 millisecond.

 

HTH

[Tim Johnson]

quote:

---

It is but that's not exactly what's happening... the new controls process so fast that they will often blow by MACRO calcs. Which if you ever goe through a MACRO in single block and it works, yet when you fun at 100% it does not work.. that's often why.

 

I was poring over some MACRO's for a Robodrill this morning for an unrelated matter and found there were numerous G4P1's all over the place where calcs were taking place. For the unitiated that's a dwell for 1 millisecond.

 

---

Is Fanuc calling/treating this as a bug?

[Grumpy Guy]

I replaced the #3006 with a M00, and the program stops and starts as it should. I am having the Fanuc guys come out and look at the machine. They think it might be a software issue with the machine.

I backed up the parameters from a machine that works and one that does not work. The parameters match pretty close, some that are different are not listed in the Fanuc book???? I will let you know what we find.

[Grumpy Guy]

Oh, and by the way I did try the above suggestions, nothing worked?