[davisboys]

Is a parameter change needed on 0i control to turn on G13 use by program O9013? If so, is it proprietary or common knowledge as it is on older controls?

[g-codeguy]

Is a parameter change needed on 0i control to turn on G13 use by program O9013? If so, is it proprietary or common knowledge as it is on older controls?

Macro call programs O9000 to O9029 (T, G, & M calls) are available for our use at no charge as far as I know.

I am not familiar with the Oi control. On the 16, 18, 21 controls O9013 is parameter 6053. On the O-TC, 00-TC, & O-Mate TC controls it is parameter 0223.

EDIT: Look in your Fanuc manual in chapter on Custom Macro, then Macro call using G code.

[chuy]

G13 is a yasnac canned cycle, I've never seen it work on a fanuc control...i believe that they have their own circular interpolation cycle.

[skullworks]

There are several different G13 commands used by control builders.

You might say Yaznaq is G13 Lite because it does not support any Z movement.

Fanuc does not support it at all, but thru the ability to assign unused G-codes (like G13) to a sub program #9xxx and pass augments (like X,Y,Z, I, J, K, F etc. BUT NOT "L") to the sub you can create a macro which is called by the G13 command just like it was a native G-code.

Haas took G13 to much greater detail.

A local shop had 2 Mori Seiki mills with Yaznaq and needed to outsource part of a job to our shop, we had a newer Mori Seiki with the MSC-518 (Fanuc 18M) control. This was a rush job. The plan was to just bring over the tooling and fixturing and run the existing programs on our mill.

Well there are a number of differences that had to be ironed out - Tapping formats etc. but the real deal breaker was his code was just loaded with G13's.

I set out to write a macro that would follow the Yaznaq method of execution. It can't be done 100% because the Yaznaq spec uses "L" in some instances and this is a reserved command letter in a Fanuc and is not directly passable.

I did manage a very well working version which had lots of error checking and grabbed values such as the last "F" and "D".

So now our Fanuc Mori runs G13 like it owns it, and we use it all the time.



Edit: - We have a very old (like 20yrs) Fanuc 0m on a Kiwa Colt 510 VMC - The machine tool builder uses a 9xxx macro sub call to handle the M6 toolchanger operation. So I think your 0i should support it as well.

[g-codeguy]

From skullworks post, it seems I may have misunderstood what you were asking. Parameter can be set up so that program O9013 can be called by any allowable G code. I thought you wanted to call it with G13.

After reading skullworks post, and re-reading yours, I would have to agree with skullworks. In order for a machine to use a special program called by G13, it would have to already be defined by the control or machine builder. Otherwise you are going to have to write your own macro, and then assign 13 to the parameter for O9013.

We have O, 11, 16, 18 and 21 controls in our shop. I am not aware of any G13 function.