Fanuc Rad error - Parameter tweak?

[Newbeeee™]

Hi all,

We have had an issue for a while when finish profiling parts. If a tolerance of +/-0.15 (.006") applies we're ok, but anything tighter then the rads shown red in the picky are always out of limit.

This is on 2x types of fanuc controls - OiMC and OiMD. They are the same machine manufacturer and model (vertical 850mm X travel).

We always run in G05.1 mode and it doesn't matter if we are running with comp or centreline toolpaths, the machine still cuts (slightly) wrong.

We are usually finish profiling with a tool only slightly smaller than the rad - so we'd use a 12mm cutter for a 6.5mm rad - so not a lot of tool movement, but the rad is obviously being generated. We would also be running a feed of around 40-60" for finishing.

The machines have been ballbarred and are all less than 10 microns.

 

So I'm thinking it's a parameter setting, angle bisection or something like?

If anyone has any ideas, they'll be much appreciated.

 

[Guest MTB Technical Services]

Ball Bar numbers, while not completely meaningless in this context, can't tell you much unless you

performed the tests at the velocity in question when machining.

 

When running in G05.1, what accuracy setting are you using? R1- R10 .

 

Not all machines run in G05.1 with a default of R5.

Without knowing what machine model you have, a best guess would be

the servo tuning and improper R value for G05.1 are the most likely culprits.

 

Questions

 

1) Machine Brand? - Yes it does make a difference as not all companies have the machine set properly from the factory

2) Linear guide or Box way?

3) R value for G05.1?

4) Workpiece placement repetition within work envelope? (Guide or way wear from repetition. Gibb adjustment can hide the problem at lower velocity)

 

It's quite possible you are fighting an inherent problem in the machine design but this likely improper servo tuning.

Get a Fanuc engineer out to the shop.

[Newbeeee™]

Tim - thanks for the reply.

Ballbar was at F1000, as that is around the usual finishing feed we use.

Job position on the table makes no difference.

The machines are linear way Chevalier QP2033 http://www.chevalier...-16-25-l_en.pdf They are extremely good value for money. We don't run a R value - just G05.1Q1 to activate, and G05.1Q0 to cancel.

I remember seeing in the old 21 control manual angles of bisection/how the control handles it, which seems more like this (possibly). But I didn't see these parameters in these new control manuals and may be barking up the wrong tree.

Yes fanuc engineer is probably the way we'll go - just wondered if anyone else had seen this before really.

[Guest MTB Technical Services]

The R value applies to ALL G05.1 operations.

When you don't specify it, it will use the default.

 

Your default value is likely incorrect for your needs.

It is now sounding like the Chevaliers are set to use R1 as the default.

This alone would explain your errors.

 

http://www.mtbtech.n...Simplified.aspx

[Newbeeee™]

Tim,

Changing parameter number 13634 (parameter to specify default 1-10) makes no difference at all.

Also, looking at the values of the other parameters around that number, I'd say the machines aren't really configured for this.

I did some testing last week and answered in another thread here:-

 

Soooooo, I dug out the yellow books and had a play this afty.

If you look in your parameter book B-64120EN/01 page 387.

Parameters 136000 onwards was what I was thinking, and parameter 13634 is the value that you set in the machine - 1= rough, 10 = accurate.

But.. we just run G05.1 Q1 in our prog call for all tools. We don't have the R value set. And we have previously servo tuned the 1768 and 1769 (acc/dec before and after interpolation in AI mode).

And the machines run sweet.

 

So I play with 13634 and make a test prog milling a square. CMM it and rad size is right with setting at 1 (rough).

Repeat with setting on 10 and no difference.

Change some of the 136000 parameters to real crazy figures and run the prog cutting air and no difference.

 

So as a conclusion, I cannot see how the 136000 parameters get activated?

Or they only do if the prog calls G05.1Q1 R#, where the R# is the activation call.

And because we don't run the R call, the lower number parameters (1768/1769) are activated and used instead?

Perhaps?

 

We previously played with 1768 and 1769 to get the machines sweet a few years ago. As the machines were set (factory default), they banged and shook all over the place when we first trialled G05.1 mode.

They do run real well for the most of the time - it's just the work has changed a bit and we're noticing this a bit more now.

[Guest MTB Technical Services]

Your AICC/AIAPC settings are not established properly.

An R value is REQUIRED for AICC/AIAPC to work at all.

Whether by using the default or specifying your own, that value must be present.

The fact that you say changing that value didn't effect anything is a clear indicator

that the machine isn't properly setup for AICC/AIAPC.

 

You really need a FANUC Engineer to come out there and tune everything properly.

[Guest]

An R value is REQUIRED for AICC/AIAPC to work at all.

Not necessarrily. This is DEFINITELY builder dependent.

[Newbeeee™]

Not necessarrily. This is DEFINITELY builder dependent.

This would make sense because when we started using it, our dealer had never heard of the need for a R value.

 

So is this builder dependant set by parameter, or builder dependand and set by the software version/options that is loaded to the machine? Just curious.

I'll give fanuc a bell Monday

[Guest MTB Technical Services]

Not necessarrily. This is DEFINITELY builder dependent.

 

James,

I understand the MTB dependency however, that default R setting either has to be a parameter or programmed.

The only other option is a value set in the PMC itself but I've never seen that done but I suppose

anything is possible.

 

Doosan has AICC on by default in every 31i series control they use.

That IS controlled by the PMC but not the R value itself.

It will always use R5 as the default value and it's specified by parameter.

You can change that default or simply specify the needed value in the program itself.

 

Running at R1 vs R10 should show a very demonstrable difference when the machine is running.

You should both hear and see the difference .

 

It looks like Chevalier either doesn't understand AICC/AIAPC or just got sloppy at the factory.

[Newbeeee™]

It looks like Chevalier either doesn't understand AICC/AIAPC or just got sloppy at the factory.

Tim - it's both

This is a piccy of how the machines were initially set up.

The boom boom boom of the machine guards changing direction had to be heard to be believed. Luckilly we didn't knock out a thrust bearing or ball screw

 

 

So 'cus it's Sunday and I'm not at work I'm still thinking about work...

It looks like it could be the 'arc radius feedrate clamp' parameters - 1730 + 1731.

I've just been swatting through yellow book number B-65270EN/06 - there's an appendix H explaining a bit about HSM

[Guest]

Tim, we sell a wide variety of machines, ALL, well all except for a couple of machines (CUBLEX and VX by option on Matsuuras) are on FANUC platform.

 

Matsuuras do use an R on old machines now you use a P, M, F, or D with values of 1~3 except D. D uses a 1 only. This goes for all 30i & 31i series.

 

Toyoda uses R by builder option.

 

Hwacheon uses R x.x The value left of the decimal controls one aspect of precision, to the right of decimal controls another using values 1~9.

 

FANUC Robos did not use an R and would alarm. You can call FANUC sloppy, i""m not making that assertion.

 

 

[Guest MTB Technical Services]

Tim, we sell a wide variety of machines, ALL, well all except for a couple of machines (CUBLEX and VX by option on Matsuuras) are on FANUC platform.

 

Matsuuras do use an R on old machines now you use a P, M, F, or D with values of 1~3 except D. D uses a 1 only. This goes for all 30i & 31i series.

 

Toyoda uses R by builder option.

 

Hwacheon uses R x.x The value left of the decimal controls one aspect of precision, to the right of decimal controls another using values 1~9.

 

FANUC Robos did not use an R and would alarm. You can call FANUC sloppy, i""m not making that assertion.

 

James.

 

Thanks for info!

I thought the P, M, F, or D word was restricted to AI-Nano.

 

I would never call Fanuc sloppy!

The most recent RoboDrill I used (with a 24k spindle and extended column) did in fact support the R value.

(It was a consignment machine from Methods)

[Guest]

All the variables are builder dependent. When an R is not allowed the default acc/dec numbers will keep a machine from alarming when a Max. load is encountered for the most part.

 

FANUC has done a poor job managing the whole AI-NANO, AI-APC, Look-Ahead, SHPCC thing. I guess in their quest to be a buffet for everyone, the number of options an combinations of options it has to be that way but sheesh...

 

Oh, an not that builders make it any better... We have some customers that have HPCC on Toyodas, it turns on with simply a G5P10000, then we have a customer with a a Feeler Bridge mill with it and it requires G8P1 to be activated before G5P10000. Oh, and nowhere in the documentation is it stated that you need to do that. Matsuura does it best IMHO, command an HON with your variable and whatever you have turns on regardless if it's AI-NANO I, AI-NANO II, or HPCC. no reason to not KIS.

[Newbeeee™]

And I thought the HON on matsuura's was a siemens thing! Every day's a school day

Thanks for the info guys

[Guest]

I want to say it started out as a Yasnac thing as Matsuuras first came with them. So I guess technically would be a Siemens thing, but works on the Matsuura with FANUC as well. When you load a program with HON/HOF in it, the FANUC converts it to G131 and if you have an R,M,F,P, or D value, it will be in there as well.

[Newbeeee™]

^^^the way they are going, they're going to run out of letters - there's only 26 - someone should tell them

[Guest MTB Technical Services]

Just to be clear about newbeeee's Chevaliers, it appears that the machines are set to use R simply because there is no alarm when it is used.

That's not a guaranty but I'm willing to guess that they are simply because of the control vintage and the company.

 

The problem appears that the machines were never properly setup and servos tuned for AICC/AIAPC at the factory.

The fact that changing the R value had no effect was a big red flag for me.

[Prodoggg]

I agree that the G8 P1 and G5 P10000 may be useful you may want to try a G61 (exact stop) we have to use it on some of our Fanucs. G64 turns it off.

[Newbeeee™]

Prodoggg - never used this as I would have thought you get squealing/cutter rub???

[Guest MTB Technical Services]

I agree that the G8 P1 and G5 P10000 may be useful you may want to try a G61 (exact stop) we have to use it on some of our Fanucs. G64 turns it off.

 

You're mixing apples and oranges.

You would NEVER use exact stop check G61 in high speed machining.

You'll always run with G64 cutting mode for HSM.

 

Typical Usage

---------------------------------------------------

Look Ahead- G08 P1(on) G08 P0(off)

AICC - G05.1 Q1(on) G05.1 Q0(off)

HPCC - G05 P10000(on) G05 P0(off)

 

FTR- The AI in AICC doesn't stand for Artificial Intelligence

It stands for Fanuc's Alpha I Series Servo System

[Mick]

Yasnac i80M on a Matsuura MC600VF... HON and HOF

 

That sure brings back some memories

[Newbeeee™]

FTR- The AI in AICC doesn't stand for Artificial Intelligence

It stands for Fanuc's Alpha I Series Servo System

Tim - every day's a school day - again!

I always thought it was the former. Our Chevalier's flash AI but they're beta drives and servos, not alpha?

The Robodrills flash as well but theyre Alpha?

[Guest MTB Technical Services]

Tim - every day's a school day - again!

I always thought it was the former. Our Chevalier's flash AI but they're beta drives and servos, not alpha?

The Robodrills flash as well but theyre Alpha?

 

Don't know about Chevalier but I got the acronym data directly from FANUC.

I would assume they got it correct but who knows.

 

FWIW- FANUC stands for Fuji Automatic Numerical Controls

[Rick46]

@ Tim Markoski I currently run a toyoda FV1680 series machine with a fanuc 18i-MB control on it. It runs the G05.1 mode with no R value after words specifying the tolerance setting. If I do put a R value it errors out in the control as soon as it reads it. this machine does hold very tight tolerances though so I assume its set in a parameter some where to 10 being the best finish. on another note I use to run a tong tai topper qvm 1100 machine with a Fanuc 18i control at another shop that had both hpcc and aicc in the control and you coud go into the settings page by navigating your way there from the offset settings button and there was a page to change the settings in hpcc and aicc from 1 to 10 for roughing and finishing. I only used hpcc on that machine but it was yrs ago and did not know you could specify the value via the post but was a useful option when roughing. My question is what or where is the parameter setting on a Toyoda machine that specifies what R value tolerance my machine is using by default because we tried to make use of the tolerance option using different R values for roughing and finishing and basically all we can do is turn it on and off no value can be set. I assume it is at 10 being the best I think that's correct anyway on the 1-10 scale if not then vise versa..lol.. thanks for any info on this..

[Newbeeee™]

Rick, not answering for Tim but I'd email Toyoda and ask specifically about your machine.

Fanuc's are so configurable every MTB sets them differently. In fact even the same MTB can set them differently from one machine to another. It can be a nightmare...