is there a way to orient the chuck at a certain angle. i know on okuma i can give it an m19 c### , c being the angle. tried this on puma 250, but nothing works.

Also, is it a safety feature that when i'm in single block i cant open my chuck. And, in a program that is a flip-op, they use m02 before m00 becasue i cant cycle the chuck that way either. this causes a double-up on parts counter. any way around this?

m19 C Probably wont work unless you have live tooling and a indexable or full C axis.

as for the chucking, use m68 or m69 to open or close it. If you want to do it manualy, from the m01 or m0 put a blank block after the stop, singleblock to it, then the chuck should work for you.

In the Daewoo Puma 240 manual, it shows M19 by itself is used to orient the spindle. The orientation angle is set by parameter 4077. You can change the orientation position by adding or subtracting degrees/4095 to the value in par. 4077.

Also, M19 can be used with an S value to specify an orientation angle. S1800 = 180 degrees, and you must be in G97 mode or you'll get an alarm.

According to the last spec I have on the Puma 240 is that Spindle Orientation is standard. Please try it and let us know.

I have also used M19 S1800 for 180degrees...

That works great in a pinch...

I think some Puma's require turning on an option bit to do M19. I think it is a 9030 number.

yeah...m19 works fine by itself but nothing i try will lock it at a specific angle. guess i'll have to do with out.... :confused:

Mdi................

G97 M19 S20 (20 Degrees)


S = # Of Degrees No Decimal
Close Chuck

Sub Spindle M119s(# Of Degrees)

P.s. No C-axis...........no Program Orient

Do You Have C-axis?

Bad Dog

Now you took all the fun out it Bad Dog... LOL!

No c-axis...:(

Well, you must have constant lead threading at least.
after the last tool stop a few inches from home in "z" then add a short thread cycle with a low spindle speed and a pitch of .360 for .720 length.
see where the spindle stops, then subtract .001 from the end position for every degree you want it to change.
you can even give it a seperate geometry offset, then bump it in z.
I used to do this and kept it as a subprogram in machine memory, then when i ran a job that needed spindle orientation for loading, i'd just call this at the end of the program.
I'm assuming you want the spindle to orientate for loading, rather than machining.

Parameter 4077 is orientation but not on the main spindle it's used to line up the live tool drive for tool changing.
Alan B

Sorry, I omitted the spindle number. #4077 S1 = main spindle, S3 = sub-spindle.

Don't change S2, as Alan says, that one's for the live tool orientation.