5 axis question

IMHO its only doing what its told...........by the prog.

what does the machine supplier say....

That sounds like a Fanuc issue, something like Look ahead, or pre-processing code. Is there a parameter for how many lines of code it can process before?

Call Fanuc directly, they may be able to help.

samurai.

The obvious stuff has already been done, I have a day or so to kill until I can get support. I was hoping someone had some direct experience with a similiar situation while I'm waiting.

Sounds more like it is waiting for a feedback response, before moving to the next position. Does it move continuously in 2-3axis moves? Sounds like a timing parameter error.

ca

..

1. I'd suggest putting a G64 before the tool path, in the off chance that the control is set to G61 (modal exact-stop).
2. Do the end-of-block interruptions occur if you drive the machine at a slower, or much slower rate? If the problem goes away at lower feeds, then you may have an issue overdriving one of your axes. It may not be a problem with a physical axis limitation, but rather an error in the parameter settings of the controller.
3. Are you licensed to use the G05 P10000 high speed machining feature of the control? Put the G05P10000 just before the first feed of the contour, and add a G05P0 at the end, and see if this corrects the problem.
4. Are you licensed to use the G43.4 and/or G43.5 functions? I am not aware of any isues with tool path interruptions with these function, but the post has to control the feed at the tool tip and not at the control point when running under G43.x. If the post is outputting G94F feeds that control the actual linear/rotary displacements, and you are driving under G43.4/G43.5, chances are you will have feeds that are both too high, and vary wildly.

That's all I can think of for now.

Good luck,

Brian.

Just a guess, but maybe the control doesn't have the 5-axis simultaneous motion option. Getting alarms when you try to program more that 3 axes in a block is a clue.

Depending on the country, the 5 axis option makes the control (and machine) export restricted, requiring special licenses and permits.

Could be that not having the option forces rotary axis motion to be positioning with exact stop (G60) rather than the continuous (G61) mode you want when doing real 5 axis work.

SteveA

What alarms?

I am assuming that by "obvious stuff" you are talking about G61, G08 and possibly G05?

Exact stop mode:

G61

The tool is decelerated at the end point of a block, then an in?position check is made. Then the next block is executed. G61 is modal, once specified it's valid until G62, G63, or G64 is specified.

Look-Ahead Control:

G08 P___ P1 : Turn on look?ahead control mode. P0 : Turn off look?ahead control mode.

Designed for high?speed precise machining. With this function, the delay due to acceleration/deceleration and the delay in the servo system which increase as the feedrate becomes higher can be suppressed. G08 must be specified in a block by itself.

High precision contour control: (option, make sure check the manual for proper use)

G05 G05P10000 ; Start HPCC mode G05P0 ; End HPCC mode

Tom

HPCC (G05) cannot be used anytime more than three axis move at a time.

Bill suggest look through the parameters it sounds like maybe one or more following error is specified at too small of a value.

You might try logging on to Anthony's chat server. There is a guy that hangs out there that is running an 18i with all the high speed and NANO stuff. He had a heck of a time getting it running correctly. Even Fanuc seemed to have problems helping him at the time.

Best, Steve

Was that the guy running a Hurco?

No not Hurco a different guy.

Not sure if anths server is running reliably but if not a co-connection can be made by logging to :

wess.mdns.org

after logging to the main then you will wanna join channel #cnc threre might not be much avtivity at any given moment depends on time of day etc but if you just stay logged then generally speaking someone will come around shortly....

Thanks for the info, I haven't had a machine with the G05 option.

Tom

No, he has a tarted up Sharp 2412. Is the shop that I visited you in keeping his Mazak busy?

Best, Steve

I use a 3 axis 18i with AICC every day. It doesn't have NANO. It does have APC. I've used 16i's with HPCC in the past.

AICC is called with G05 like this:

G05 Q1 R1 (thru) R10 G05 Q0

Q = on/off R = precision - 1 is loosest 10 is tightest.

APC, which is good for 2D contouring is called like this:

G08 P1 (on) G08 P0 (off)

HPCC:

G05 P10000 G05 P0

The difference between HPCC and AICC is HPCC is hardware based (RISC processors - expensive) and AICC emulates HPCC with software.

I'm sure Bill has that covered though since he explained most of it to me a couple years ago, the rest I got from Sam.

You're sure it's not ot G5.1?

Only if it's a GE Fanuc. The Japan Fanucs I've worked on have 1,2, and 3.

Very.

Now that you made me actually check, yes, that's what it is. I set up a Mastercam post to control it with misc values.

And unlike HPCC, which is hardware, AICC - the software version - works properly when any combination of axis motion is commanded.

It also isn't avalable on a machine with Nano interpolation as far as I know. The two would be redundant. That doesn't mean some dunce hasn't done it, however.