Fanuc 15m "G05.1"

[Slick]

I have read up a little on the "G05.1" command for the older style Fanuc control. The newer 16i was a lot easier to comprehend. I was hoping somebody out there could give me a run down in english (control manual reference).

From what I can gather, and correct me if I am wrong, the output shoud be "G5.1" followed by a "P" value.

 

Here are some things I am confused about:

 

Is the "P" value supposed to be a range from 1-10000? i.e "G5.1 P1000" or is it similar to the 16i where it needs to be preceded by a G990 setting and the "G5.1" is just activating it?

 

If the value is supposed to be a value, 1-10000, what do you suggest running? I am happy with the "Semi-finish" setting of the 16i.

 

G code placement. How should an output string look?

 

G0 G90 X_ Y_ M3_

G5.1 _?

G43 _

G1 Z F_?

 

Any and everything you coud explain on this would be great. I have sipped the code in to my code and experimented, but would like to understand what I am actually doing.

[Guest CNC Apps Guy 1]

Ok, you are confusing two functions for starters.

 

G5.1 if followed by a Q1 (and depending on the builder, possibly an R value) ex. G5.1Q1 R1 (roughing), G5.1Q1 R10 Super Precision Finishing. This function started off being called SHPCC, but now is known as AI-NANO I. It can have from 180 Blocks to 1000 Blocks look ahead. 1,000 block look ahead is a hardware option. 200 is a software option.

 

G5P10000 is also known as HPCC or AI-NANO II. This has 1,000 block look ahead as well as as short as .4ms. This is a hardware option.

 

Using MPMaster, you will get correct formatting. Brett and I did some work together on this.

 

HTH

[Rick Henrickson The Boeing Co.]

We just use the G5.1 P10000

[Chris Rizzo]

What James said.

 

Lots of differences in how the control/machine is setup.

 

on our 18i we use:

 

G49

M300 Q1-5 (specs what level of ai, 1-5)

G5.1 Q1 (Q1 turns it on, Q0 turns it off)

 

you gotta look in your machine manual and included fanuc info to figure out how it really works for your machine.

[Rick Henrickson The Boeing Co.]

yeah my bad james is right G5P1000

[Slick]

So you output the G5P1000 one time at the top of the file? Is G5P0 the cancel feature? I have the manuals for the 15m right next to me, just not a lot of reading time at the moment.

 

Are you running a 15m control Rick?

 

Thanks James!

[Zoober]

On our 16i, G5P10000 turns on. Yes it is on until a G5P0.

Be careful, you can't switch between G93/G94 when active, and other caveats.

[Rick Henrickson The Boeing Co.]

I think the 15, 16, 18, 21, and 310 all use the G5P10000 if you have the option,

[Guest CNC Apps Guy 1]

You can't just turn it on at the top of your program and turn it off at the end.

 

It shoudl be turned off at the end of each tool. Also, you'll need to issue a G49 to cancel your ht. offset or else you won;t be able to turn it on again.

 

Now with all that said, by parameter, it is possible to have it running all the time so you won;t have to worry about turning it on a and off. BUT !!!CAUTION!!! consult with your Machine Tool Dealer/Builder PRIOR to enabling this as it may have unintended consequences.

[Slick]

Okay, so Ithink I have enough to start. I'll be messing with it tomorrow morning to see what works.

 

I wish I would have had the G49 tip two days ago James! That was fifteen minutes of troubleshooting I could have done with out. The one note my manual doesn't mention!

 

So I haven't searched this next one, but since I am doing R&D this weekend:

 

How about the G10.3/G11.3 High Speed setting? This one looks a bit more complex...

[Zoober]

James, I use HPCC G5P1000 and do not use a G49 in our programs. Now we are using Niigata's tool mgmt macros, but I don't remember seeing one in there either.

What all can happen without it. Is it a safety thing I should be adding?

[Guest CNC Apps Guy 1]

Here's where each machine tool builder's implementation of controls and function usage causes things to get a little dicey. (I'm sure you're groaning about now). In about 50% of the applications where I've used G5.1Q1 and higer orders of High Speed Functions (HSF), they needed the G49 to properly cancel the HSF. I personally do it 100% of the time as it DOES NOT negatively affect anything (unless you call the G49 too early; in which case it would cause a crash). I have it here,

 

code:

---

G1 G40 X.7805 Y3.8928

G0 Z3.785

G5.1 Q0

M5

G91 G28 Z0.

G90

G49 (<<<<<<<<<)

M1

---

and have NEVER had a problem yet on Mori, Toyoda, Matsuura, Mutsui Seiki, SNK, Kitamura and a few others that escape my mind currently.

 

HTH

[Newbeeee™]

Robert,

If you don't use G49 and your code works ok, then you may have a G49 in the toolchange macro?

 

As CNC Apps guy says, it's waaayyy safest to put one in, as this will (should?) then work on any other machine.

 

Slick

G05.1 cannot run in canned cycles (tapping/ drilling etc) so must not be called for these ops.

However, an alternative maybe G08? This is lookahead only, but does give 'deceleration before interpolation'. So, to me it is a form of contour control, although Fanook UK will only say it's look ahead?

Anyway, this can be called at the start of a prog by G08P1, and then cancelled at the end of the prog by G08P0.

This may be a simpler option for you, as it can be active for canned cycles.

 

Personally, we haven't had any luck with either, as we get a very rough finish on the bottom of pockets where the machine interpolates (looks almost like the head bounces in the z). It is good on a straight move though.

It is obviously a parameter thing, but we haven't got to the bottom of it yet...

[Guest CNC Apps Guy 1]

High speed functions should not be used in canned type cycles IMHO (even if they are capable as in G8P1) There is no benefit to using it. If you use MPMaster, it will not post out on OPCODE 3 type paths (Drilling type).

 

G8P1 is the least sensitive of all the High Speed options. It has the least amount of parameters to control it also. It's better than nothing AS LONG AS IT"S BEEN SETUP PROPERLY parameter-wise.

 

G8P1 is best suited for prismatic types of parts.

G5.1Q1 is best suited for more complex types of parts (but not really molds or implantable body joints and the like)

G5P10000 is for the most complex, massive quantities of data with small moves per block type stuff. You won't see any real advantage having G5P10000 unless you're running the right kinds of parts.

 

HTH

[Newbeeee™]

James,

Have you ever run a test piece to see any difference between the different options?

I'm thinking flat plate aerospace type ribs and 'simple' scan work (like the shape of a pc mouse).

The sort of work we do is the above with a +/- .005" tolerance, so for the scanning we use the mcam filter to output G2/3 moves, rather than 1/4million lines of G1's.

With our OiMC controls, we can accurately feed very quick, but we are going to run a test piece with some unfiltered (G1) code, and see just how bad the control chockes up.

Cheers

[Slick]

I agree with you on the G49 James. The shop I'm at now had a standard Safety line at the beginning of every tool call out:

 

"G0 G17 G40 G80 G90"

 

I am changing the post's this week to:

 

"G0 G17 G40 G80 G90" I'm thinking this way is better just because it's more visible before the "G43" call out.

 

I will try the G5.1 P1 on my next part. In this part I am doing some live 4th axis cuts. Would this be the case where a G5.1 P1000/10000 would be applicable?

[Guest CNC Apps Guy 1]

quote:

---

...Have you ever run a test piece to see any difference between the different options?...

---

Yes. On more occasions than the example listed here; Linky

 

quote:

---

...The sort of work we do is the above with a +/- .005" tolerance, so for the scanning we use the mcam filter to output G2/3 moves, rather than 1/4million lines of G1's...

---

Regarding filtering, there is a relatively small cycle time difference (when compared to the % of code increase) See link above.

 

quote:

---

...I will try the G5.1 P1 on my next part. In this part I am doing some live 4th axis cuts. Would this be the case where a G5.1 P1000/10000 would be applicable?

---

It's not really the number of axes or amount of data per se that determines what tu use. The biggest deterining factor IMHO is average block length (distance moved per block). If you only have an average block length of say .001, that is going to be a very dense program, and you're going to NEED all the control processing horsepower you can get your hands on. You may have a programmed feedrate of say 250IPM but depending on the control and options, you may only get to say 50IPM max. I'm just throwing ball park numbers out there but you can pretty much calculate all that stuff to figure out your maximum achievable feedrate. There's more to High Speed Machining than most people think. On top of all that, there may be surface finish requirements that may be a higher dictate than the other factors.

 

HTH

[DavidB]

Good read,Cheers James the Fanuc god

[Guest CNC Apps Guy 1]

Thank you for the kind words, but I still have PLENTY to learn.

 

Actually next week I'm going to be doing some HSM testing between G5.1Q1 and G5P10000 for cycle time differences, surface finish differences, and full 4 Axis cutting, etc... Hopefully anyway. We're still waiting on GE FANUC to show up with the hardware, which should happen Monday (here). But it will be a good exercise nevertheless.

 

Man I love my job. Shhhhhhhh, but I can't believe they pay me to do what I do. Man I scored the smokin' job.

[Guest CNC Apps Guy 1]

Ahhh, found the formulas for calculating MAX possible feedrate based on block length.

 

F= D X 60 X 1000/E

 

Where:

 

F = feed rate in in./min. D = distance between data points E = block execution time in ms

 

 

So a 1ms BPT(which is getting close to the fastest processor you can purchase) with a block length of .0001 (yes extreme I know) would be able to run a max feedrate of 6 IPM. .001 would yield a 60 IPM Max f/r and .010 would be able to run a max of 600 IPM and so on and so forth.

[DavidB]

James would the F = units/min?

If not whats the caculation for metric?

 

Cheers

[YoDoug®]

James teh smart guy in the room, when he speaks its wise to listen.

[Thee Dragracer1951]

I remember the original post James did on the G8's and G5.1's Great info. I usually use G8's but may start looking at G5.1's. As I understand it, in my 0iMc control with AI Nano, I have 120 blocks of look ahead controled by G8's and I think 40 blocks using the G5.1's. I'll have to go back and look at the book...

[Guest CNC Apps Guy 1]

AFAICT it is Inches per minute, in which case you would take the above calculation and multiply the feed rate x 25.4

 

.4ms is the fastest I've seen on a FANUC spec. (yes that is point four milliseconds)

 

One last thing, after you do your math to figure out what your maximum feedrate is, you should remember that just because your control is fasat DOES NOT mean your machine, it's drive system and it's mechanical properties will actually allow it to execute that fast. Acceleration/Deceleration before/after interpolation all play a role in determining what the net result at the part level will be.

 

HTH

[Zoober]

quote:

---

just because your control is fasat DOES NOT mean your machine, it's drive system and it's mechanical properties will actually allow it to execute that fast.

---

In addition to that, just because you have the HPCC (or whatever HSM), does not mean that your machine is properly setup.

We had to have Fanuc in for over a week to tune our 5x Niigata that had HPCC, but had never had the drives tuned. Our C axis was even setup for the wrong gear ratio. We didn't know, because it had scales, and positioned good for 3+2, but couldn't keep up in full 5x work.

 

Furthermore, I was told by the Fanuc tech that they can tune the drives differently for different applications of HPCC. You may want to have the system tuned to YOUR most common application.

James - Please correct me if I'm wrong.