Need Help!- I fix em, not program them-much

[underthetire]

So, have a OLD lathe, was retrofitted a few years back with a Fanuc 21i (GE). Operator/programmer was trying to use a G71 roughing cycle, looked correct to me, but was only doing one pass to finish size. I changed to a G73, and the roughing cycle worked, although the book shows more of a copy cycle, it looked just like a G71 does. Same values all around, just altered the G71 to a G73. The G70 line does not run the finish pass at all. Tried a G71 in place of the G70, and it switched the machine to metric?! Am I missing something or do we have corrupted software or something else i'm missing. Been on Fanuc controls for 20 years, but mostly just basic programs and fixing them.

[dcoupar]

Can you post the program here so we can see it?

[underthetire]

Originally Posted by dcoupar Can you post the program here so we can see it?

I can, i'll try to get it up tomorrow. Almost beer thirty.

[stevo1]

I don't have the manual in front of me but there is a parameter setting for using G70 and G71 for inch and metric instead of G20 and G21. I came across this on a 15series I was setting up a few years back and never knew it existed until then. Took me a few days of digging until I figured it out. I am not sure if the 21i series has this parameter but based on what you stated I would almost bet that is the issue. IIRC it was under the section of programming/edit.

Stevo

[sinha_nsit]

Originally Posted by underthetire ...Operator/programmer was trying to use a G71 roughing cycle, looked correct to me, but was only doing one pass to finish size. ... Same values all around, just altered the G71 to a G73. ...

Possibly depth of cut is too large.

Difficult to believe. Syntax is different. Post your program.
It was possibly a G73 cycle which somebody "modified" to G71. Is it one-block or two-block format?

[underthetire]

Originally Posted by stevo1 I don't have the manual in front of me but there is a parameter setting for using G70 and G71 for inch and metric instead of G20 and G21. I came across this on a 15series I was setting up a few years back and never knew it existed until then. Took me a few days of digging until I figured it out. I am not sure if the 21i series has this parameter but based on what you stated I would almost bet that is the issue. IIRC it was under the section of programming/edit. Stevo

That sounds correct, and actually makes complete sense. When they did the retrofit, they had done 2 others just before this one, both with15 controls. I'd bet they tried to keep them the same. Double checked format again, ran the G71 as typed on a newer lathe. The control seems to take single or double line G7* commands without issue.

[stevo1]

Make sense to me but I was not able to confirm it as I could not find the 21i manual in my archives (sucks). But if you program G71 and your machine switches to metric that makes sense to me.

Stevo

[sinha_nsit]

I do not have the manual in front of me, but IIRC, G70/G71 select the mode in G-code system B and C. G20/G21 are for system A only.

[underthetire]

Well, lloks like parameter 3401.6 and .7 control that. I'll play with it today and see what I come up with.

[sinha_nsit]

I just checked.
G70/G71 select mm/inch mode in G-code system C.
In system C, G71 of A and B, changes to G73.