fanuc 18-m high speed option g code

[dforsythe]

Anyone knoe what the G or M code is for a Fanuc 18-M high speed / look ahead. I was told we have the option. this is for a early 90"s Awea Bridge mill.

 

thanks, damian

[Guest CNC Apps Guy 1]

Try G5.1Q1 in MDI. If you don't get an "Improper G-Code" alarm, that's what you want to use.

 

You turn it on before you turn on your TLO. Turn it off G5.1Q0 before you zero return Z. Then coMmand a G49 after you zero return Z Axis.

 

HTH

[Jasond0530]

If G5.1 dosn't work try G8p1 works just as well as the g5!

 

HTH

[spade117]

Advanced Preview Look-ahead - G08 P1(on) G08 P0(off)

Artificial Intelligence Contour Control - G05.1 Q1(on) G05.1 Q0(off)

High Precision Contour Control - G05 P10000(on) G05 P0(off)

[dforsythe]

Thanks for the info. I will give it a try when i get back from vacation. One more thing. the reason i ask is the control / machine is choking on code when finishing. i just did a large Lam tool about 72" x 8" and mastercam said the cycle time for the finish tool was about 11 hrs. they let it go all night long and it was only half way done the next day it ended up being 23 hrs total. The tool path was Hybrid step over set to .012 with toll set to .0004, create arcs and smooth random. the program feed was 130 ipm but the fastest i saw the it hit was about 45 imp with a lot of 20-30 ipm.

 

 

 

Thanks for the help, Damian

[Guest CNC Apps Guy 1]

You NEED to be using some sort of look ahead with cycle times like that.

[K2csq7]

it ended up being 23 hrs total

 

What kinda material is the part?

[dforsythe]

What kinda material is the part?

 

6061 with a .750 ball em we usually prog upwards of 300 ipm on the haas while finishing. the 90's Model Awea's have a hard time with the code so we prog them at 50% of normal. It has to be a perfectly staigh cut of over 5" to get up to 130 IPM.

 

I will try some of the other codes today. thanks for the help

[dforsythe]

the control takes the G5.1 Q1 and flashes aicc at the btm. we will give it a shot today. thanks

[Matthew Hajicek - Singularity]

Was looking to the same thing today, found this thread and this instructional PDF:

http://www.compumachine.com/Support/Tech-Bulletin/How-to-use-AICC.pdf

 

Followed the PDF and it seems to be working great.

[Surface]

I don't understand why a feature which allows the machine to run faster and more accurately needs to be turned on.

Who has ever said, "My machine runs too fast." or "What can I do to increase corner rounding errors?"

 

So why doesn't the machine automatically turn this feature on?

[Joe788]

Was looking to the same thing today, found this thread and this instructional PDF:

http://www.compumachine.com/Support/Tech-Bulletin/How-to-use-AICC.pdf

 

Followed the PDF and it seems to be working great.

 

I word of caution to anybody following the directions on that pdf: BE CAREFUL OF THE G49! The pdf example is showing the G49 being called before the zero return. On a lot of machines, this will try to ram your spindle nose to your work offset Z0. in the blink of an eye. Never a good situation.

[Matthew Hajicek - Singularity]

I don't understand why a feature which allows the machine to run faster and more accurately needs to be turned on.

 

Because it's deviating from exactly following your instructions. Some people may not want the machine to think for itself. Also notice the R1 - R10 in the PDF, which adjusts from more smooth to more accurate.

[Cannon]

Because it's deviating from exactly following your instructions. Some people may not want the machine to think for itself.

 

These kind of people should not be using cnc machines at all. The machine is following the program more accurately and faster with look ahead turned on, who would not want that?

[Mic]

Because it's deviating from exactly following your instructions. Some people may not want the machine to think for itself.

 

These kind of people should not be using cnc machines at all. The machine is following the program more accurately and faster with look ahead turned on, who would not want that?

 

More accurate yes, faster no.

 

Because of the more accurate path control the machining time will in most cases also be longer because the controller slows down the feedrate to stay on the correct path.

 

I've done some test on new Matsuura's with 30i/31i and the fastest running time was without highspeed active. But this was very unaccurate so it could only be used for roughing.

[Newbeeee™]

The only thing I'll say to this is in my experience, cycle times were quicker. This is on chevalier VMC's with oimc controls.

We tuned the parameters so we could use g05.1 and it averages around 10% cycle time reduction (6 mins per hour).

The profiles are as accurate as before but the machine is constantly moving, where before (in std mode) the tool would look like it paused/dwelled when profiling (albeit it didn't stop because finishes were always good).

There are different parameters that g05.1 uses, and different algorithm as well, and the machine motion definately looks smoother when running it.

So we run it all the time on all jobs.

[Guest CNC Apps Guy 1]

In my tests, cycle times were quicker as well with High Speed active but that depended on what R level was active. It started tipping slower around R6 IIRC. It's been a few years since I've run the tests. It's probably time to run them again.

[Newbeeee™]

We have never ran with an R value. I don't even know if our machines would take it - never tried.

But they're happy running with just the g05.1 call.

[Mic]

In my tests, cycle times were quicker as well with High Speed active but that depended on what R level was active. It started tipping slower around R6 IIRC. It's been a few years since I've run the tests. It's probably time to run them again.

 

I tested a 3X Volumill program on a Matsuura MX-520 with iZ-1/30 ( Ai Contour Control-II ) Programmed feedrate was 7200mm./min. and Highfeed 20000mm./min.

 

Mastercam backplot time 4m36s

G131 R1 time 7m 5s

G130 ( no highspeed active ) time 5m32s