SILLY FANUC

[SledGeek]

I know it's hard to beleive, but occasionally we need to hold and reset a program,on the card for editing ,for a Oi-mc When I have the G5.1 Q1 in the program , it won't restart the machine without a "5111 improper modal g-code (G05.1 Q1)" alarm. I have tried to end the modal with the G5.1 Q0 command , manually , but no dice. I've done it at the machine and thru the card. I have to shut it down and restart to clear it.

 

Can anyone share another way to cancel this without shutting down ?

 

Thnx

[MikronGuy]

cutter comp is still active. generate a G40 in MDI.

[SledGeek]

didn't work.......anything else?

[MIL-TFP-41]

These 2 lines in MDI

 

G40 G49

G5.1 Q0

 

That order works on one of our machines here. Something about canceling after the height offset is canceled IIRC

[Guest SAIPEM]

These 2 lines in MDI

 

G40 G49

G5.1 Q0

 

That order works on one of our machines here. Something about canceling after the height offset is canceled IIRC

 

%
O9020 (CUSTOM M-CODE FOR AI-NANO PROCESSING RESET)
(SET PARAMETER 6080=490)
(USE M490 VIA MDI)
G40 G49
G5.1 Q0
M99
%

[Guest CNC Apps Guy 1]

Yes G49 is the key to cancelling AICC/AI-NANO.

 

Command a G91G49;G90 in MDI and you can restart.

[SledGeek]

Thanx fellas -that worked. It's just the G49 that it needs. I guess I figured it would need the Q0 in there for cancelling Q1. If I ingle step at the beginning and don't let it read the tlo after the AI APC, it's fine...will start right back up. I miss my the 16i with HPCC.....can't wait for a new machine.

Never came across this until i started trying to tune this thing and kept shutting it down mid prgrm......

Fanuc in their infinite quest to nickel and dime , has made it more confusing to run some of there controls.

I did find some good info tho, in case any one is interested . It clearly dfines the different forms of AI and packages that the manual can't do. And specifies a crap load of parameters to tune.

 

 

 

Oi tuning

[Newbeeee™]

Hey Sled, glad you liked my post. Glad to be of service

It's probably out of date now after the release of the 0iMD version

 

Since writing the post, we've tweaked parameter 1771 (now 180) and parameter 1768 (now 66) due to the awesome (overly used word nowadays, but very apt in this instance) new dynamic/high speed toolpaths mcam now has.

We're routing with 14mm knuckle form cutters at 7metres/minute feeds now and on 'value for money' (read cheap) chevalier machines with the 'economy' (cheap) Oi control.

If we had the money for a Matsuura 38krpm FX2, it sure would be a hell of a lot of fun

[SledGeek]

Hey Sled, glad you liked my post. Glad to be of service

It's probably out of date now after the release of the 0iMD version

 

Since writing the post, we've tweaked parameter 1771 (now 180) and parameter 1768 (now 66) due to the awesome (overly used word nowadays, but very apt in this instance) new dynamic/high speed toolpaths mcam now has.

We're routing with 14mm knuckle form cutters at 7metres/minute feeds now and on 'value for money' (read cheap) chevalier machines with the 'economy' (cheap) Oi control.

If we had the money for a Matsuura 38krpm FX2, it sure would be a hell of a lot of fun

 

 

You guys did some homework there The only way it goes outta date is if you HAVE the MD lol. I'm in the same boat for right now, trying to get every last tweak to make up for "economy". Pretty frustrating when u r not used to economy. We are looking at Makino's and Okuma's though

All I have is the AI APC, which best I can tell, is xtra look ahead only, so I spend alot of time creating the smoothest simplest path I can . The worst is free form stuff that cuts nicely until you get to the intricate portion of the geom..... Trying to finish hardmill forms at a reasonable sfm and maintain chip load becomes frustrating

Oh well, I like challenges

[Newbeeee™]

In a previous 'life', we had all singing all dancing hitachi's. 16i controls awith lots of look ahead but couldn't accurately contour above a metre a minute, becuase the parameters were not set-up.

If you're looking at new machines, I'd specify on the purchase order that the thing must accurately contour at X feed rates. Just becuase the control option is there, it doesn't mean the MTB has set it up.

[SledGeek]

In a previous 'life', we had all singing all dancing hitachi's. 16i controls awith lots of look ahead but couldn't accurately contour above a metre a minute, becuase the parameters were not set-up.

If you're looking at new machines, I'd specify on the purchase order that the thing must accurately contour at X feed rates. Just becuase the control option is there, it doesn't mean the MTB has set it up.

 

 

That's one of the reasons we r looking at Makino. 2 miles away with excellent lifelong support from SST. Got, got, got ,got no time to be messin around eatin up run time Gotta support foreign and American presses/dies to keep profit sharing up..... i mean keep presses runnin

[Guest CNC Apps Guy 1]

...Fanuc in their infinite quest to nickel and dime to maintain THEEEEEEEEEEE most reliable control on the market...

Fissed for accuracy.

 

When functions are activated, they all have their different requirements to shut them off. Maybe your machine tool dealer did not take the time to explain this. More confusion comes about because of poor training from machine tool dealers.

[SledGeek]

Fissed for accuracy.

 

When functions are activated, they all have their different requirements to shut them off. Maybe your machine tool dealer did not take the time to explain this. More confusion comes about because of poor training from machine tool dealers.

 

Hands down my favorite control, been running them for years. Doesn't mean they don't charge alot to turn things on. Not knockin em , by any means. I've have learned you just need to be very specific about exactly what your expectations are.On the training portion you are right. We didn't get any training with this particular control cuz we inherited it with a company we bought. Some of the training I've been to at Fanuc leaves something to be desired as well. There's just so many variations of controls over the years , it becomes a bit of a pain to keep track. But, by the same token, their ability to customize per user is unrivaled.

 

Apparently, my frustration with not knowing this control inside and out yet, is.... well......apparent

[MIL-TFP-41]

Gotta love Fanuc's secrecy....I have read stories about their plant in Japan...the place is tighter than Ft. Knox. Then I have had more than one Fanuc tech stumped and because Fanuc has this crazy hierarchy it took days to get the problem solved rather than minutes.

[shazam/TPP]

These 2 lines in MDI

 

G40 G49

G5.1 Q0

 

That order works on one of our machines here. Something about canceling after the height offset is canceled IIRC

 

the G49 before the G5.1 Q0 is this correct? i ask because the link sledgeek posted shows opposite

 

Again, don't call in a drill or tap cycle.

G05.1Q1 MUST be called before the G43 line.

G05.1Q0 MUST be called to cancel it.

G49 (tool height comp cancel) MUST be called after G05.1Q0. If you don't call G49, you cannot call/activate G05.1Q1 again (and the yellow books don't tell you this).

 

is it the same for an 18iMB control? we received no training in this and the manual is ... well you know

[SledGeek]

the G49 before the G5.1 Q0 is this correct? i ask because the link sledgeek posted shows opposite

 

 

On mine, I just had to mdi G49 because I never let it read it at the end of program ...because of stopping midway thru.

[Guest CNC Apps Guy 1]

I've alwys called the G49 after cancelling AI-NANO/AICC out of habit. Never had any issues. RObodrills REQUIRE G49 to even do a tool change so, it's in there for me always regardless of AI-NANO/AICC's condition.

 

I read through that link above. There's some good info in there. I disagree about the whole G8 is better than G5.1 arguement though. Just because you can turn somethign on at the beginning of a program and off at the end does not mean that's the best thing. You have more tuning optins with G5.1, you have higher look-ahed possibilities with G5.1, etc... There is no good reason to use those functions for drilling and tapping. Those are NOT processor intensive tasks. Of course G8/G5.1 F**K up threads. You're affecting acc/dec, you don't want that when you're tapping, you want the speed and the feed totally in sync. Other than that, he had good info.

[Newbeeee™]

I've alwys called the G49 after cancelling AI-NANO/AICC out of habit. Never had any issues. RObodrills REQUIRE G49 to even do a tool change so, it's in there for me always regardless of AI-NANO/AICC's condition.

 

I read through that link above. There's some good info in there. I disagree about the whole G8 is better than G5.1 arguement though. Just because you can turn somethign on at the beginning of a program and off at the end does not mean that's the best thing. You have more tuning optins with G5.1, you have higher look-ahed possibilities with G5.1, etc... There is no good reason to use those functions for drilling and tapping. Those are NOT processor intensive tasks. Of course G8/G5.1 F**K up threads. You're affecting acc/dec, you don't want that when you're tapping, you want the speed and the feed totally in sync. Other than that, he had good info.

 

To be clear on the G05.1 V G08 thing.

It all depends upon what the MTB has specified, as there are two levels of G05.1. Ours had 'lookahead' G05.1 apparantly. The next level upgrade has lookahead with contour control.

Now I assume thats a different algorithm (James - can you confirm as I always wanted to know?).

But our 'lookahead' only version with no 'contour control' seemed to be contradicted by the yellow book, as this states that the G05 lookahead has 'deceleration before interpolation'. Well to me, if it's slowing before cornering then, it is contour control???

 

The Robodrill was another thing. Spent a couple of days on this...We found out the G49 toolchange thing and ended up modding our post to always call it at the end of each tool.

The robo's have a compiled toolchange macro that can't be changed. We even created a 9000 toolchange macro program with the G49, called it in the parameters (activated by the M6 tool call), and disabled the compiled toolchange macro by paramater, and the 9000 version just wouldn't call. The machine just carried on using its own macro. There's another thread on Practical Machinist about that as well

 

James - By memory, I think you can call the G05 on a Robo for drilling and tapping (not that you would) and the machine reads it but just ignores it (parameter setting?).

We wanted to initially call the G08 at the start of the prog, because we could easily hard code that into our post ourselves.

The G05 was above our ability. So this is what I meant by 'easier' (for me anyway )

However, Phill at 4D (our dealer) modded the post so for all milling ops only (ie not driling/boring/reaming/tapping), G05 is always called. And like I said, it works out average at 6 mins per hour cycle reduction running it. Per machine (4 of them). Every day. Just for a line of code at the top of the tool call.

Cheers