Fanuc 5 Axis Options

[Greg Williams]

Hi All,

 

I am looking at a Matsuura LF-160 for make specialist high tolerance gears. I think I just about have the spec down pat but I am wondering if somebody may be able to tell me what these options actually do. And more importantly will they change the actual path that the cutter takes?

 

- NANO smoothing Software

- Tilted work Command (Is this the same as G68?)

- Work Setup Error compensation G54.4

- Tool posture control

 

Thanks for your help

[Reko]

Hi Greg, I'll take a stab at this with the preface that I am a bit of a rookie on this particular controller.

 

NANO Smoothing is an accelerate-decelerate algorithm so it should only affect surface finish, not accuracy.

 

Tilted work plane is similar to G68 (rotation), but G68.2 (TWP) can define any arbitrary plane in 3D space. It uses IJK to define a first, second, and third rotation. With this function, you can still use regular 2-dimension functions like cutter comp and drill cycles because your plane is actually moved to make the Z-axis normal to the plane you are machining.

 

WSEC is for fixture error and can be used if your part's rotation is off.

 

I have not used G43.4, tool posture control, but I'll watch this thread for more details.

 

HTH

[Guest MTB Technical Services]

You'll want to make sure you get G68.1 at the very least for 3D Coordinate conversion.

You're probably better off getting G68.2 for the simplicity of using a single line of code with the Euler Angles (I,J,K).

You really only need it if your spindle head is nutating.

 

G54.2 is commonly referred to as Dynamic Fixture Offset.

It was original designed for large horizontal boring mills where it would be impractical to use the center of rotation as the part origin.

This function allows you to comp out the distance between your actual center of rotation and where you have it set.

This is strictly 3+2 positioning only.

 

G54.4 Work System Error Compensation is what you want if you need true 5-axis simultaneous motion.

 

G43.4 is commonly referred to as TCP or Tool Center Point management.

It's more common to see it used on 5-axis machines with Nutating heads as it automatically compensates for the gage length of the tool.

You don't need to have your post handle the gage length calculations if you use TCP.

Be very careful using it on a VMC with a trunion as it is designed to maintain the tools position in relation to the workpiece.

It can easily cause your slowest rotary to reach max feed almost instantly.

 

Accelerate/Decelerate options do effect accuracy.

 

AICC and AIAPC have settings specific to accuracy so it's very important to use it properly.

With a linear motor machine, the tuning will be entirely different than a conventional linear-guide or boxed-way ball-screw machine.

(G05.1 Q1 for contour control and G05.1 Q3 for AI-Nano)

 

FANUC AI High-Speed Modes - Simplified

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

[Guest]

NANO Smoothing is an accelerate-decelerate algorithm so it should only affect surface finish, not accuracy.

Not true. It absolutely affects accuracy.

 

WSEC is for fixture error and can be used if your part's rotation is off.

Not only rotation but position as well. WSEC has 8 axes it works with. x, y, z, a, b, c, A, and B (or whichever rotary axes your machine has). The non caps letters are the amount of error in each axis, the capital letters are the angles at which the error measurement was calculated at. You HAVE to have this option is you want to comp for error in simultaneous 4/5-Axis movement, but it works great for 3+2 as well. Personally, I'd never go the RTDFO route on a machine capable of simultaneous 5. It limits what I can do. I don;t like unnecessary limitations.

 

Like Tim warned; TCP on a trunion style machine can create some issues. Seen it first-hand. We have a customer with Nutating Head machines and Trunion machines. They took a program from the nutating head machine and put it on the Trunion machine and had some unexplainable gouging. The A-Axis was at 180% velocity We ended up having to crank the High Speed Look ahead accuracy all the way up to get it to slow itself down enough to stop the gouge. It was an interesting excercise. Vericut did not show the gouge or give us any indication there was a problem in that area but when I brought the program into CAMplete, it did indeed show me the axis velocity spikes which then helped us figure out the solution. So, be careful with this one. It's powerful and can do some amazing things, but it can also be hair-raising to watch.

 

will they change the actual path that the cutter takes?

All these options have the ability to affect positioning in one way or another be it how fast the smoothing allows an axis to reach it's programmed position, or how IJK Vectors are calculated. Hopefully you will get CAMplete with the machine. That will save you a load of grief on the posting side.

[Greg Williams]

Guys,

 

Thanks for your responses, This clears up a few of my questions.

[Greg Williams]

It seems that CAMplete is only offered to the US market. In the UK they offer IPS which looks like an on board collision checking system. Has anybody tried it?

[crazy^millman]

Greg ICAM can help you with the post if you would like some information about it. Shoot me an email and I will be gald to assist.

[Guest]

It seems that CAMplete is only offered to the US market. In the UK they offer IPS which looks like an on board collision checking system. Has anybody tried it?

 

We have yet to see a machine with it yet. I've seen a few technical briefs but nothing I can disclose. Interesting about CAMplete not being offered in the UK. They offer it in Japan from what I've been told. You guys have somethign else over there that someone is trying to protect?

[Watcher]

Tim and James!

 

Thanks for making this place a great source of information and hands on experience. I always learn something from you two in an often basis.

[Sticky]

That is a pretty zippy little machine! 3500ipm rapids and a 46,000rpm spindle

[Guest]

That is a pretty zippy little machine! 3500ipm rapids and a 46,000rpm spindle

What is even more impressive than that is the acceleration. Hang on to your hats!

[Greg Williams]

We have bitten the bullet and ordered it, Looking forward to seeing this baby run.

[Guest]

You've got mail Greg.

 

Oh, please don't share. For you and your company's eyes only.

[Greg Williams]

OK Thanks

[Prodoggg]

I have a Fanuc 31i-A5 control on a vertical 5-axis machine. We are new to 5-axis and I'm not sure when to use G43.4, G5 P10000, G5.1 Q1 R#, G8 P1. Also we have been using G54.2 P#, RTDFO, and I read in some threads that G68 may be a better option. What are your thoughts? Can I use G54.2 and G43.4 at the same time?

[Guest]

Since you're new to 5-Axis, I would highly, no, check that, HIGHLY recommend spending some time with your machine tool builder/dealer AE. That time will be time WELL spent.

 

G5P10000... if you have this use this on everything except drilling. It is HPCC. On occasion, I've seen some builders require G8P1 be activated prior to G5P10000.

 

G68 is Coordinate Rotation. WAY different from G54.2 Px

 

AFAIK you can't use G54.2 Px and G43.4 at the same time.

[Prodoggg]

thanks

[Prodoggg]

Since you're new to 5-Axis, I would highly, no, check that, HIGHLY recommend spending some time with your machine tool builder/dealer AE. That time will be time WELL spent.

 

G5P10000... if you have this use this on everything except drilling. It is HPCC. On occasion, I've seen some builders require G8P1 be activated prior to G5P10000.

 

G68 is Coordinate Rotation. WAY different from G54.2 Px

 

AFAIK you can't use G54.2 Px and G43.4 at the same time.

Thank you for the info. Check that, instead of G68 I meant G68.1 and G68.2. Do you know anything about these functions and how they may be used in conjunction with G43.4?

[Guest]

G68.2 is Tilted Work Plane, Essentially you are telling the control you are positioned, rotated and or tilted about a given position and using vectors to define it.

G43.4 is TCPC a 5-Axis function.

 

They can be used in conjunction with each other but here's where it gets too long winded to explan how, why, when, etc... in a forum so I would HIGHLY recommend you contact your MT Dealer/Builder for further explanation. Some things are MTB specific as well and TPC is one of those options where on a trunion type machine the consequences incorrect usage can be devastating to the machine.

[Prodoggg]

Thank you for your time.

[Guest]

My pleasure.