5 axis machining with FANUC?

Hi.
I have always been under the impression that when doing 5 axis simultaneous machining, you had to program the part with the work offset coordinate positioned in the center of the rotational axes, and that you had to regenerate and repost your program for every setup if you were unable to clamp the fixture at the exact same position every time.

I talked to some guys running DMG machines with Siemens controllers yesterday, and they said the Siemens controllers had a "Traori" function that could keep track of the work coordinate when the 4th and 5th axis rotated, so you could program 5 axis parts with the work offset placed somewhere on your part and it would stay at the same position on your part even if you rotated the tables and the tool axis changed.

I have worked only with Fanuc controllers and have not seen any mention of such a function.

Does anyone know if the Fanuc controllers can do this?

Yes they can....They call it TCPC...Tool Center Point Control. G43.4 if memory serves. dunno when they started using it...but I do know that it is on their 30i/31i controllers

We have that exact problem with our old Kitamura Supercells with Fanuc 15MAF.
Everything needs to be re-posted when you move an offset.

CAM systems don't support tool cutter comp with 5 axis cycles either, so you have to update your CAM system with exact cutter sizes as well if you are doing any profiles which are very tied up.

I think only the latest generations of Fanuc controls (eg: 310 / 32) supports TCPC

If you are thinking of buying a 5 axis machine I would go Heidenhain
(although it loathes me to say it, they are the best for 5 axis)

Who did you talk to at DMG? I know that the Siemens control in my experience is WAY better than a Fanuc. I think that people are just used to Fanuc over here in the states. But, when you start to use a control like the Siemens or I heard Heidenhein is even better, you really start to see how limited the Fanuc control really is!

I tried to find some info on Fanuc´s center point control, but didn´t find much. It seems pretty cool though. Anyone got a link for some info on this?

The guys I talked to were DMG salesmen. I got the impression that the Heidenhain control probably was the best choise if you did very complex work, but the Siemens control was a lot easier to learn if you were used to a Fanuc.

I'm following this thread with great interest. We are considering the purchase of a 5 axis Robodrill and I'd assume Fanuc is the only choice of control.

We've just got a 5 axis VMC with a Heidenhain 530i control
and that does the co-ordinate system change when you do a 4/5th rotation as well as having the tcpm thingy

Its quite a nice control now heidenhain brought in some decent flexible cycles and multiple work datum settings.

Boris

<<<annoyed because the owner's son has hogged the thing all week... but fun when the instructor put an AL hogger in there and profiled a part at 200"/min and everyone went "**** me thats fast" and I went "ahh almost a 1/2 reasonable feed rate"

I think the chances of the RoboDrill being offered with anything other than a Fanuc Control is nill to non existant !

The RoboDrill is a fantastic bit of kit, but VERY restrictive in USEABLE travel in a 5 axis setup, you not only have the number of tools to limit you but taking into account you need long tool holders to get at sides of a part being held in a baby chuck / vice and then a small Z travel, you can get very stuck.

It's fine if you have a long term job you know will fit, but for a jobbing shop it is just to restrictive.

(we almost bought a couple last year and went into this in some depth)

If you want the super high speed DMG 5 axis machine they (used to maybe this has c hanged recently) only offer it with Heidenhain.

GF (Mikron) or Mazak would be where I would spend my money for a budget (<£180,000) 5 axis machine and Matsura for mass production multi-pallet machine.

I would avoid Hass for full 5 axis, apart from it being so slow and has many control issues, you have only got to talk to any high end CAM vendor to find a list of disapointed customers, who expect to do Mazak Variaxis or Mikron quality work on their Hass with a trunion table and realise they can't.

It depends on if you wany to machine multi-face valve blocks or mould tooling.
Your £60,000 5 axis Hass will be fine for valve blocks.

barbter said:

Basically, if it fits in your hand it will go on the machine no probs. Anything bigger and you'll have to look into it.

Click to expand...

This statement says SO much. Thanks for the input. We will check out the alternatives, keeping in mind that Haas will probably come in the cheapest but wouldn't necessarily be my first choice.

Even if you choose Mazatrol, Fanuc, Siemens or Heidenhain control unit, you need a proper postprocessor in order to use full capacity of control units.

Using TCPC (or TTPC) in 5-axis machining brings flexibility as you all mentioned, but more importantly, this feature increases the machining accuracies due to the advantage of controlling tool tip point instead of controlling pivot (rotation) point of the rotary axes. Using this feature will prevent unwanted small gouges that occur beause of uncontrolled tool tip.

However, using TCPC (or TTPC) is not always the right choice, since this feature has its advantage mainly in 5-axis simultaneous machining.

While performing indexed 3+2 axes milling and drilling operations, using TCPC will bring some restrictions. On some control units, circular movements are not allowed in TCPC mode, and on some others, drilling cycles are not allowed in TCPC mode.

Plane rotations are the most proper way of performing 3+2 indexed milling and drilling operations. It is better not to use TCPC feature in this kind of machining operations.

A proper postprocessor is the one that automatically sorts the type of machining operation (3-axis, indexed 3+2 axis or 5-axis simultaneous) and generates codes accordingly.

Visit our web page to see some special algorithms that are developed to form more advanced postprocessors.

www.manusncsoft.com

Denim said:

Hi.
I have always been under the impression that when doing 5 axis simultaneous machining, you had to program the part with the work offset coordinate positioned in the center of the rotational axes, and that you had to regenerate and repost your program for every setup if you were unable to clamp the fixture at the exact same position every time.

Does anyone know if the Fanuc controllers can do this?

Click to expand...

The Fanuc 31i on the RoboDrill has an option you can purchase called G54.2 dynamic offset. This option eliminates the need to program from the center of rotation. I have used this on 3 + 2 but not with contour milling.