Need Help!- Thread Milling using "C" axis no "Y" on the machine

[tejano4life72]

Hello,

I am a swiss programmer and I don't know a thing about Mori Lathes. I want to try to program a thread mill on a Mori SL-25m. This machine does not have "Y" axis. So I would like to see if anybody out there knows if I can use "X,Z & C" to do so. I have done it on a L20 citizen machine. This Mori SL-25m is about 10 years old. I was wondering if anybody out there has done it and if so if they can please help me out by pointing me on the right direction.

Thank you.

[underthetire]

Depends on the machine vintage, and that machine is 15+ years old. SL25m's were replaced in the mid 90's by the three digit machines. Ser# might help, and control type.

[littlerob]

Absolutely yes, even if the machine wouldn't support it (I would be very surprised if it doesn't) you could find the toolpath and post out tiny incremental moves. UTT will correct me if I'm wrong.

[tejano4life72]

the machine type is: SL-25MC5 and it has a Fanuc Series O-T control

[underthetire]

Ok, so it's a 20 year old machine, if it's green it's older still. It may or may not be able to, the very first ones had either C axis position only, or optional C axis contour control. First you need to command C axis mode and see if it will feed positions, or just index to positions.

[tejano4life72]

UTT yes it is green. How about SL-253 BMC/500 control MSG-501 (18i-TA) or a SL-25 M0 control MF-T6. If so, would have an example program I can see? I dont have any manuals for these machines.

THANK YOU

[the thrill]

first thing you'll want to do is enable the C axis and try to do a G1 move with Z and C at the same time to see if you have C axis contour or position only. I'm going to use a program technique from the newer model machines as i'm not 100% familiar with the programming on such a vintage machine

M69(SPINDLE UNCLAMP)
M45(MILLING MODE)
G28H0 (HOME C AXIS)
G1G98H360W1.F5000. (MOVE C 360 DEGREES AND Z 1.0 INCREMENTALLY AT A FEED OF 5000 DEGREES PER MNUTE)

if that test passes, you have a contouring C and can continue forward.

if it's a center hole, you can just simply position X to the center of the hole, do a linear move and turn on cutter comp to the diameter you wish to machine, rotate c and move z at the same time (H360 or -360. W = the pitch you wish to machine i.e. for 1/4-20 W.0555 or -.0555 depending on if you want to machine out of the hole or into the hole from current position.

example:
M45
G28H0
G0T101
S2000M13
Z.25
X0M8
G1G41G98X.25F10.
H360.W.0555F2000.
G40X0F10.
G0Z.25
M5
M9
M1



if it's an off center hole, use polar interpolation (g112/g12.1) and program it in the same manner as X/Y movements remembering that polar interpolation automatically converts degrees per minute into inches per minute.

[CNCRim]

Originally Posted by the thrill if it's an off center hole, use polar interpolation (g112/g12.1) and program it in the same manner as X/Y movements remembering that polar interpolation automatically converts degrees per minute into inches per minute.

Have you try?