Fanuc look ahead question

[Thee Dragracer1951]

I have a new machine with a Fanuc 0iMc control

I bought it with 120 blocks of look ahead in order to contour and surface at higher feed rates. Could someone please give me an explaination of how to get this to work? I have been reading the manual and it tells me to use a G8. An examle of some code would be wonderful. That way I could go about getting my post to output correctly.

Thanks

[Psychomill]

Here's an example of code:

 

N1G0G17G40G80G90

T1M6( 1.0 CARB EM )

G55X-3.1Y3.S12000M3T1

G43H1Z.1M8

G8P1 (Turn on lookahead)

G1Z-.5F200.

G41D9X-2.5F480.

X2.5

G2X3.Y2.5J-.5

G1Y-2.5

G2X2.5Y-3.I-.5

G1X-2.5

G2X-3.Y-2.5J.5

G1Y2.5

G2X-2.5Y3.I.5

G3X-1.734Y3.3572J1.

G1G40X-1.6697Y3.4338

Z.1

G8P0 (Turn off lookahead: optional)

M9

G0G91G28Z0M5

G91G30X0Y0

M30

 

 

G8 can be specified nearly everywhere. The main condition is that you specify it in a block by itself. Most machines utilize "G8P1" to turn it on, then "G8P0" to shut it off. "Reset", M30 and such will also default the machine back to off.

 

A few notes.... Most machines will need to have the G8 mode shut off for several things like canned cyceles (tapping, drilling, etc), High speed skip, polar coordinate interpolation, etc. It should continue to work for things like rotaion (G68), mirror image, etc. I normally don't ever have G8 shut off in a program unless I'm drilling and tapping. It's also good to have it called up in the main for every tool you use it on after toolchange. That way, if you restart a program, you're in G8 if you need it. Then also add a G8P0 to your canned cycles in the MC post file.

 

[Thee Dragracer1951]

Awesome. Thanks, That was a lot clearer than the Fanuc manual.

I'm on it!

[connormac]

I have look ahead but if I try to go faster than 75 ipm the machines seem to try to start cheating corners.

[Guest CNC Apps Guy 1]

Here's my sample I show everyone.

 

 

G49G94

N1T1M6(1/2 FLAT ENDMILL)

G8P1(LOOK AHEAD ON)

(MAX * Z5.)

(MIN * Z0.)

G0G90G54X.5Y6.63B0.S20000M3

G43H1Z5.M8

Z1.1

G1Z0.F1180.

G41D1Y7.13

G3X0.Y7.63I-.5J0.

G1X-13.535

Y-7.63

X13.535

Y7.63

X0.

G3X-.5Y7.13I0.J-.5

G1G40Y6.63

G0Z5.M9

G8P0(LOOK AHEAD OFF)

G91G28Z0.M5

G90

G49

M1

 

I add the G49 because many of my machines have AICC/AI-NANO and they require the G49 before you call it again.

 

In my posts I created 2 postblocks. phsmon and phsmoff. In those postblocks I turn on and off the appropriate contour control algorithm. I use a Misc. Int. and I have them on ALWAYS with the exception of opcode3 cycles (canned cycles). My post logic checks for the condition of the opcode in the postblock.

 

HTH

[Psychomill]

quote:

---

I have look ahead but if I try to go faster than 75 ipm the machines seem to try to start cheating corners.

---

I should have asked this to Dragracer as well... but what machine are you on? Was the Look ahead part of the original install or optioned later (Connarmac)?

 

Some machines just plain have a hard time going fast. Even if the lookahead is set properly, there some that just "can't get out of their own way". This has to do with other issues like axis drives, motor types, guideway types, screw pitch (which brings up pitch comps, accel/decel capabilities), etc. You can have some adjustment by means of parameters for servo drive, vector comps (for angle of motion) to try and boost the acceleration and accuracy in the corners. It's a game of trade-offs. But these things can screw up your machine in a hurry so I do not suggest someone with the lack of this type of adjustment experience to start messing with these parameters. It could take some time (even for the experienced) or it could be as simple as tweaking a few things in with a Ball-Bar.

 

Code-wise, some machines may force other criteria. As with James' machines with AICC/AI-NANO, he has to use certain codes to meet certain conditions. G8 is also not the same as G5 for criteria. G5 has a couple other "requirements" for use.

 

For the most part, on the dozens and dozens of machine brands/models I've used G8 on, the "factory" settings were adequate. Some I've had to tweak in with a metrology guy or factory support. A couple machines were just simply "hopeless" and only used it to force finish accuracy and constant speed (which was at the least, "some" improvement over the original state).

 

[Guest CNC Apps Guy 1]

Each type of "Look Ahead" has certain types of work it is suited for.

 

G8P1 - 2-2 1/2 Axis work is where Look Ahead is best suited. It can help with 3D programming but it just does not have the speed to keep up with large amounts of data and small moves.

 

G5.1Q1 - 2 1/2 - 3 Axis Work is where AI-NANO 1 Shines. It has more look ahead capabilities, it processes faster than Look Ahead and can better cope with large amounts of data with small moves.

 

G5P10000 - HPCC (On older controls) AI-NANO 2 (On newer 31i Controls) is most definitely suited for detailed Moldwork. Huge amounts of data with very small moves. This is a hardware option that involves RISC Processors. If you do Moldwork, this is the option for you. You won't really see any benefits doing 2-2 1/2 axis work with this option.

 

G6.2 - NURBS This option requires the above option to be installed as well as it is also a Hardware Option involving RISC Processors. It is most definitely suited for Mold and Die work and is a relatively rare option. I think in the field I've only seen it in a handful of shops, then again, I don;t get into a whole lot of Mold Shops so I may be totally out of line. You'll also need some additional software like Metacut Pro to convert your Point to Point Program to NURBS. Not sure on the pricing but it's easy enough to get a quote from Northwoods Designs for it.

 

Now, if I had the option of having these options installed at the factory or in the field, I'd take the factory because at the factory, they'll be set for the machine with the basic settings. Now you can have your machine tuned by a Factory Fanuc rep that will absolutely make your machine sing and is worth every penny on the investment but it's not cheap and takes some time (a day or two last I checked).

 

HTH

[Guest]

thanks a ton James,

been asking this question for some time-fanuc reps-tool sales persons-ap engineers etc. and you gave the best description i have heard yet.

 

love this forum

 

Doug

[TheePres]

James,

I have seen options of Q1-Q4 using G05.1, would you please explain the difference on these options.

Also, how is it possible to turn on AICC in middle of a program, if i insert anywhere but on 1st tool I get alarm.

[Thee Dragracer1951]

This is on a brand new Sharp 2412s with a Fanuc 0iMc control with the look ahead installed at the factory

The G8 helped a TON! It also has AI contouring (G5.1)

This is a little box way machine that I bought for cutting all the stainless I seem to get loaded with...

[heavychevy2155]

How do you like your Sharp, does it sound good when cutting stainless?

[Guest CNC Apps Guy 1]

Thank you for the kind words Doug. I try to be as helpful as possible whenever possible.

 

quote:

---

...I have seen options of Q1-Q4 using G05.1, would you please explain the difference on these options...

---

These are acc/dec settings that differ from builder to builder.

 

Q1 may be one machine's "Super Finish" Settings while it may be another's "general" settings. It just depends.

 

With Super Finish parameters enabled, expect to run slower but you'll get phenominal finishes and accuracy.

 

With the roughing set of parameters, expect the machine to haul you kno what but still maintain a relatively decent accuracy spec. The machine may be a little too jerky for some people's liking but if I want speed and I'm roughing... I can put up with a little sheetmetal rattle to get it done faster and better.

 

Then the other settings fall somewhere in between these two.

 

The 0i-MC is not a bad control at all. Not as fast as the 16/18/30/31's but will definitely get the job done for most things. I have one attached to a Fanuc Robodrill MATE in the showroom right now and I've played with it a bit. I think the functinality has a lot to do with t what the builder puts into it. Since the Control Builder is Fanuc and the Machine Builder is Fanuc as well... it's loaded to the hilt with options.

 

quote:

---

Also, how is it possible to turn on AICC in middle of a program, if i insert anywhere but on 1st tool I get alarm.

---

It's not being turned off properly. Look at my sample above... do it EXACTLY like that and it will work. You are probably not canceling the height offset (G49). Notice after my toolchange I do that? That's just in case I need to reset the machine, I can do restarts at the tolchanges and the machine will be in the necessary condition to start AN-NANO.

 

HTH

[Thee Dragracer1951]

Interesting thoughts on controls James.

I upgraded my Sharp from a 0i mate control as I wanted to do fourth axis stuff with it. They offer a Fanuc 18m control on their larger machines but not this one so I did wnat I could...

The machine sounds just fine when cutting stainless. I do some heat exchanger plates, head and return connectors... in 316 stainless. Lots of pockets that are .75 deep. I ramp in nad pocket at .2 deep a pass at 200 sfm and .004 per tooth. The machine sounds just fine. It'll take a bigger cut but the end mill won't

I've been using ProMax Varatec variable helix four flute and they work pretty well but I'd like to go faster.

In fact...if anyone has any suggestions about endmills in 316, I'm all ears

[DavidB]

With my Makino I have to turn on SGI (HPCC) with a G05 P10000 and it has to be after the G43 line.

 

I also have to turn it off at the end of every tool before the G91 G28 Z0. move.

[Fred from Université de Sherbrooke]

We have all the options possible on our Fanuc 31i control. (AI contour, NURBS, 3D circles, ...).

For our 2-2 1/2 works, should we only use G8 P1? Or do we have any advantage of using others options. We're doing a lot of 2D stuff, with a lot of very very small details in plastics. So we need good details definition (corners) and very high feed rates. Any suggestions? Thank's

[Guest CNC Apps Guy 1]

You can use the others there's just no real advantage to it as there usually is not enough data/small enough moves where you would see a difference in cycle time, but if you have very small moves and a lot of data (such as a surfacing program) that's when you see noticable differences.

 

Personally, I run AI-NANO (or whatever the highest order of contour control I have on the machine I hapen to be running at the time) always.

[Cannon]

We have a Hartford vmc with 18i control and factory installed AICC. It runs really slow in corners on G5.1 Q1, so I tried to change it G5.1 Q2 and G5.1 Q3 but it just alarmed "improper G- code". Is it that they have not installed these settings in factory or am I doing something wrong?

[Guest]

I might be wrong but I thought the only options for the were Q1. on and Q0. off

[Cannon]

If you read the thread someone asked a question about Q1-Q4 and James Meyette answered that these are different acc/dec settings.

[Guest]

Like I said I might be wrong,

 

I stand corrected

 

[Guest CNC Apps Guy 1]

Q1 is ON and Q0 is off. On SOME machines they use different Q settings but if you get an alarm then your machines does not.

 

There are a group or parameters that affect acc/dec that you can modify IF you know what they are AND IF you know what you're doing. If you have to ask yourself "...if..." then you don't and you should not. Sorry to be blunt, parameters are not for screwing around with, if you do not know EXACTLY what you are doing. You can turn your $1,000,000 machine into a boat anchor in a few keystrokes if you don't know what you are doing. Call your local machine tool dealer and have an AE come and help you. That's the best advise.

 

[ 01-22-2007, 11:03 AM: Message edited by: James Meyette ]

[Post dept]

All,

 

I have been working on adding some of this functionality to mpmaster for everyone to use. I'll be sure to document everything very well so it can be used as a reference. I'm having a problem though.....I don't have a machine.

 

If you've got some time to help, it will be beneficial to everyone.

 

 

Here are a couple of questions that I've got:

[DavidB]

Brett happy to help you.

 

I added this to my MPmaster.

code:

---

 phsmon               # High Speed Machining Contour Control On

if opcode$ = 3 & mi8$ > 0, mi8$=0

#if mi8$ = 1, pbld, n$, "G08 P1", "(LOOK-AHEAD ON)", e$

#if mi8$ = 2, pbld, n$, "G5.1Q1", "(AICC ON)", e$

if mi8$ = 3, pbld, n$, "G05 P10000", "(SGI ON)", e$ #DAV WAS HPCC

prv_mi8 = mi8$

lookahead_flg = 1

!mi8$

 

 

phsmoff #High Speed Machining Contour Control Off

#if prv_mi8 = 1, pbld, n$, "G08 P0", "(LOOK-AHEAD OFF)", e$

#if prv_mi8 = 2, pbld, n$, "G5.1Q0", "(AICC OFF)", e$

if prv_mi8 = 3, pbld, n$, "G05 P0", "(SGI OFF)", e$ # DAV WAS HPCC

lookahead_flg = 1

!mi8$

 

pbld, n$, "G43 H1", pfzout, scoolant, e$ #dav

phsmon #DAV High speeed machining options

---

Thanks to John aswell for his help.

[Guest]

quote:

---

Thanks to John aswell for his help.

---

Thanks David but the "REAL" thanks go to James and his coding.

 

[DavidB]

Yes Thanks James. I guees everyone knows he is the Fanuc guru