Hi guys, and gals. (have to not be sexist)
I have had a Wickman 52-200 cnc lathe for about 2 years now,
it came with live tooling but it always tripped out after a couple of seconds running,
so i didn't bother with it as i never had a use for it,
However i have recently accuired a job which i would like to usu it on.
i found a siezed bearing on the drive shaft and replaced it,
but i have never known ho to engage the c'axis
i justneed to engage it and then drill some cross holes around the diameter,
if anyone could tell me which codes engage the c'axis and rotate it that would be a great help.
it has a fanuc ot control on it!

thanks again,

Deejay.

It probabally depends alot on how the OEM set the C axis up, whether or not the spindle motor itself is used or if there is a separate servo for the C, which is disabled when the spindle is running.
If you got the lathe new 2 years ago you should be able to get the info from the OEM, if not, hopefully someone has the same lathe, as the Fanuc manuals will not tell you.
Do you have the OEM operators manual?
Al.

hi al
thanks for your reply,
i do have the manual but all that tells me is that m19 engages references the spindle.
which it does,
but then i don't know how to index it.

FOR MORE DETAILED AND COMPLEX WORK, YOU NEED TO FIND OUT ALL OF THE PROPER PROCEDURES IN RUNNING YOUR LIVE TOOLING. BUT TO GET STARTED YOU CAN TRY OUT SOME SIMPLE FACE AND CYLINDRICAL DRILLING. M19 SPINDLE ORIENTATION SHOULD NOT BE USED HERE!!! HERE IS A SIMPLE PROGRAM THAT IS COMPATIBLE WITH FANUC 18i CONTROLS AND SHOULD BE SIMILAR TO YOURS. JUST SUBSITUTE WITH PROPER M-CODES. THIS PROGRAM DRILLS 4 EQUALY SPACED HOLES ON THE OD OF A 3.00 SHAFT.


N6;
(.250 HSS DRILL);
G28U0G30W0;
G00 T0606;
G54 M76; (C-AXIS MILLING MODE);
G28 C0;
G50 S1200;
G97 S1200 M3;
G00 X3.100 Z.100;
M08;
G00 Z-1.500;
M50; (C-AXIS BRAKE ON)
G98 G01 X2.0 F14.00;
G00 X3.100;
M51; (C-AXIS BRAKE OFF)
G00 C90.;
M50;
G98 G01X2.0 F14.00;
G00 X3.100;
M51;
G00 C180.;
M50;
G98 G01 X2.0 F14.00;
G00 X3.100;
M51;
G00 C270.;
M50;
G98 G01 X2.00 F14.00;
G00 X3.100;
M51;
M05 M09;
G00 Z.100;
G28U0G30W0;
T0600;
M01;

OF COURSE CANNED CYCLES,SUB-PROGRAMS, AND MACRO CAN BE USED.JUST START PLAYING AROUND WITH IT AND FIND ALL INFO YOU CAN FROM THE MACHINE TOOL BUILDER.
GOOD LUCK!!:)

hi al
thanks for your reply,
i do have the manual but all that tells me is that m19 engages references the spindle.
which it does,
but then i don't know how to index it.

If M19 works referencing the C axis, then did you try e.g. G1 C90 F5 command to see if rotates to 90°?
Al.