What's new
What's new

Fanuc O-TC and G54

gregormarwick

Diamond
Joined
Feb 7, 2007
Location
Aberdeen, UK
The O-TC does not support additional work offsets (not even as an option AFAIK), instead relies on work shift.

G54-G58 do not exist and alarm out when you try and enter them.

However, it is somehow aware of G54 as it's clearly set as a default at startup, it's right there in the list of active modals.

Is there any way to prevent this control from alarming out when it encounters a G54? It's the only real hurdle in being able to use a single unified post for my O-TC and our Oi-TC.
 
The O-TC does not support additional work offsets (not even as an option AFAIK), instead relies on work shift.

G54-G58 do not exist and alarm out when you try and enter them.

However, it is somehow aware of G54 as it's clearly set as a default at startup, it's right there in the list of active modals.

Is there any way to prevent this control from alarming out when it encounters a G54? It's the only real hurdle in being able to use a single unified post for my O-TC and our Oi-TC.
Hello gregor,
I suspect that the alarm being raised is p/s010. That being so there is no parameter solution I'm aware of, but there is a fudge you could use. Register the number 54 in whatever parameter that is available between 6050 and 6059 to create a Custom G Code, G54. Lets say 54 is registered in parameter 6050, create a program under the number O9010 that contains nothing other than M99 to return control to the calling program. When G54 is encountered in your program, program O9010 should be called and immediately return control to the Block following where the G54 in the calling program was encountered.

Regards,

Bill
 
Hello gregor,
I suspect that the alarm being raised is p/s010. That being so there is no parameter solution I'm aware of, but there is a fudge you could use. Register the number 54 in whatever parameter that is available between 6050 and 6059 to create a Custom G Code, G54. Lets say 54 is registered in parameter 6050, create a program under the number O9010 that contains nothing other than M99 to return control to the calling program. When G54 is encountered in your program, program O9010 should be called and immediately return control to the Block following where the G54 in the calling program was encountered.

Regards,

Bill

Very clever Bill!

When the machine is finished it's current job I'll give that a go and let you know how I get on.

Alternatively, that solution might be somewhat confusing to the operator, so I might have to live with two posts. We'll see!

Cheers.
 
Very clever Bill!

When the machine is finished it's current job I'll give that a go and let you know how I get on.

Alternatively, that solution might be somewhat confusing to the operator, so I might have to live with two posts. We'll see!

Cheers.

Hello gregormarwick,
It should be no more confusing than the program encountering a G54 and not raising an alarm. If the O9000 Series Programs are protected and hidden via parameter, as they should be, the operator will not be aware of the Macro Program being called by G54. It will seem that the program reads G54 and advances to the next Block.

Regards,

Bill
 
Have you checked with Fanuc? I believe it is an option for turning but rare. Fanuc options must be purchased and loaded like Okuma does. Gone are the days of merely flipping a parameter.
 
Hey Brent,

If you want to know, post up the firmware version and I'll look in my info and see if it shows up.

Kevin

Hey Kevin,

I wouldn't even have any idea where or what to look at to tell you what version it is? Not the first clue? Lol...

How do you tell what version of firmware it is?

Brent
 
On the 0 series the firmware number shows on the screen for a moment when you boot the control. Sometimes if the CRT is a bit slow to warm up you won't have a chance to see the number before it is gone. If that happens just turn the control back off, count to 3 and turn it back on. Usually that will let you catch the number.
 
Not exactly sure what it is so this is what I saw. It ain't up there long that's for sure. Lol...

Freaking sideways picture wtf?

Brent

20190419_003724.jpg
 
No not that I'm aware of. It's a "C" axis lathe but none of the tooling came in with it so we've never used it. I'm almost positive it doesn't but maybe I need to look it over better. Can't imagine where I'd find it I've been all through it.

Brent
 
Can you shut it off by parameter? What I mean is not to load the conversational programming when it boots up at startup? Hell maybe its shut off? The danm thing comes on almost instantly.

Brent
 
Mine is a 669. I set 916.2 and lo and behold I now have work offsets. They look exactly like Brent's - hidden behind a toggling softkey. So thanks all for that!

Next question is, how do they work? There is no Measure soft key like on the Oi, and MZ doesn't work like when setting the work shift. There must be an easier way than calculating the offset and entering it directly?
 
On this particular machine that's exactly what I do. I've never got this figured myself. The guy in post 6 has a detailed description on how to use the measure function but I was unsuccessful when tried it on my machine. Maybe I wasn't doing something exactly right? Maybe he'll show back up here?

Have a look below. Talk about finding a needle in a haystack! Lol

Brent

Problem getting my head around work offsets on lathe
 
Next question is, how do they work? There is no Measure soft key like on the Oi, and MZ doesn't work like when setting the work shift. There must be an easier way than calculating the offset and entering it directly?

Hello gregor,
If your control has User Macro and you let me know how you're setting Tool Geometry, I can give you a Macro Program for setting the Work-shift Offset value of the Offset of choice.

Regards,

Bill
 
Maybe I should start a new thread, but my question logically follows some of the discussion here. Another member (wakeless foil) and I are beginning to use a Nakamura Slant Jr. CNC lathe with Fanuc 0-tc software, version 0662-08. So we don’t have access to G54-59. Fine. Previous owner we can’t contact due to anonymity of the auction environment was making parts with this machine. It works completely, no errors or anything when we check individual functions. All parameters are there.

We’d like to get started with baby steps and we’re both new to CNC so we’re studying Peter Smid v.3 and watching some Titans videos, waiting for Nakamura op manual to get here, have downloaded about 5 Fanuc s/w manuals that apply to 0-tc.

Anyone have some short programs on file that will run on our “stupid” 0662 s/w version? Wakeless has succeeded in communicating via RS232c so it’ll be easy to dump part programs in. Machine came with ample tooling.
 
Last edited:








 
Back
Top