What's new
What's new

Looking for Programming insight - Fanuc 0T lathe

bengineer08

Plastic
Joined
Jun 17, 2022
Location
Northern KY / Cincinnati area
Hi, I'm trying to teach myself how to program my early 90's Miyano lathe (Fanuc 0T). I'm hoping someone might have some insight into what's going on. More than likely it's a syntax error or something. Or maybe the control is older than the examples I've dug up and repurposed, and it doesn't like the order of things or something? I've got a couple quirks I can't figure out.
First, when I start the program, it'll go through the first few lines and get to the tool change line, change tool and just hang up there (no error or anything). Cycle Start won't start it going, but still no error. I can hit reset, but then it skips the line immediately following the tool change. If I hit reset, then switch to edit and back up to the line that was skipped, I can hit cycle start and it seems to run ok.
Second, I was trying to turn a fillet at the back using Z-25.0, R1.0; and it didn't seem to like that at all. If I take the ", R1.0" out it'll work just fine (but, of course, no radius). I understand there are other ways to do the fillet, but would this control be too old to do a simple "Z-25.0, R1.0;"?

N1 (ROUGH TURN);
G40;
T0101 M06; (<this is where it hangs up)
G50 S2500; (<this is the line it skips)
G96 S250 M03;
G00 X28.0 Z5.0;
G01 Z0.1 F0.1;
X-0.2 F0.05;
G00 X 28.0 Z2.0;
G71 U1.0 R1.0;
G71 P100 Q200 U0.2 W0.05 F0.2;
N100 G00 X19.0;
G01 G42 Z0.0 F0.2;
X20.0 Z-0.5;
Z-25.0, R1.0; (<-this is where if I remove the ',R1.0' it runs fine)
X26.0;
N200 G40 X28.0 Z5.0 F10.0;
M05;
G97;
M30;

Any help to tips would be greatly appreciated. Thanks.
 

wmpy

Hot Rolled
Joined
Dec 16, 2011
You don't use M06 on a lathe. Take it out, and it should read the line fine.
 

wmpy

Hot Rolled
Joined
Dec 16, 2011
I've only seen the ,R syntax used on Hardinge lathes. Try taking out the comma, and run the line

Z-25.0 R1.0

If it still doesn't work as desired, then you may need to do as 706jim suggests and use G02.
 

DouglasJRizzo

Titanium
Joined
Jun 7, 2011
Location
Ramsey, NJ.
Hi, I'm trying to teach myself how to program my early 90's Miyano lathe (Fanuc 0T). I'm hoping someone might have some insight into what's going on. More than likely it's a syntax error or something. Or maybe the control is older than the examples I've dug up and repurposed, and it doesn't like the order of things or something? I've got a couple quirks I can't figure out.
First, when I start the program, it'll go through the first few lines and get to the tool change line, change tool and just hang up there (no error or anything). Cycle Start won't start it going, but still no error. I can hit reset, but then it skips the line immediately following the tool change. If I hit reset, then switch to edit and back up to the line that was skipped, I can hit cycle start and it seems to run ok.
Second, I was trying to turn a fillet at the back using Z-25.0, R1.0; and it didn't seem to like that at all. If I take the ", R1.0" out it'll work just fine (but, of course, no radius). I understand there are other ways to do the fillet, but would this control be too old to do a simple "Z-25.0, R1.0;"?

N1 (ROUGH TURN);
G40;
T0101 M06; (<this is where it hangs up)
G50 S2500; (<this is the line it skips)
G96 S250 M03;
G00 X28.0 Z5.0;
G01 Z0.1 F0.1;
X-0.2 F0.05;
G00 X 28.0 Z2.0;
G71 U1.0 R1.0;
G71 P100 Q200 U0.2 W0.05 F0.2;
N100 G00 X19.0;
G01 G42 Z0.0 F0.2;
X20.0 Z-0.5;
Z-25.0, R1.0; (<-this is where if I remove the ',R1.0' it runs fine)
X26.0;
N200 G40 X28.0 Z5.0 F10.0;
M05;
G97;
M30;

Any help to tips would be greatly appreciated. Thanks.
OK.
Most turning centers don't use an "M06" for tool change, they use a four to six digit T code.
Such as "T0101" - the first two digits are the turret station number, the second two are the offset number.
The G50 S line should always be first., right after the "O" number.
I rarely use G41/G42 cutter comp in a cycle, I prefer to use it on the finish tool only. When cancelling I usually use a G40 with a single axis pull off perpendicular to the part surface.
Your feedrate - IPR or IPM?

I have some great two axis manuals I wrote when I worked for Doosan. I'd be happen to send them to you. PM me.
 








 
Top