Need Help!- Okuma OSP Tapping Cycle

[pyropainter]

Hello, we have an Okuma OSP 500-LG Lathe. I am trying to program a tapping cycle for a 1/4-20 tap. I am not much of a G Code programmer and for the most part use Virtual Gibbs when programming. Our post doesn't seem to work. When it comes to special operations like this we change the program manually. The manual is old and the pages containting this information have been lost . Your help is greatly apreciated.
Barry

[stevo1]

can you post the code that is not working?

Stevo

[pyropainter]

I will see what I can do. You probably won't see anything from me until sometime Thursday afternoon. Thanks for the response.
Barry

[Thawk53]

Example 20 T.P.I.

(Right Hand)
G0G95G97X30.Z30.S375T0101M42M3M8
X0.0Z1.1
Z.25
G77X0.0Z-.5F.05
G0Z1.1
X30.Z30.M9
M1


(Left Hand)
G0G95G97X30.Z30.S375T0101M42M4M8
X0.0Z1.1
Z.25
G78X0.0Z-.5F.05
G0Z1.1
X30.Z30.M9
M1

[pyropainter]

I did try the program that thawk32 offered. At G77 my machine gives me "G" code unavailable error. Is it possible my machine will not tap?
Barry

[underthetire]

I will for sure not rigid tap. Should be a floating tap cycle available, but the 500 was kind of a striped down 5000. I'll see what I can dig up.

[underthetire]

No tap cycle listed other than G77. Think you will need to program it using G1 and a proper feed in inches per rev. Remember to use a floating holder.

[pyropainter]

I do have a tap holder that appears to move under tension. Does this program look like it would work for a 1/4 20 tap. I realize that the tap will have move under tension as it completes the cycle. I have seen others on this web site talk about 5 or 10 percent less than then greater than the pitch of the tap. What do you think about this program? Thank you.
Barry

(Right Hand)
G0G95G97X30.Z30.S375T0101M42M3M8
X0.0Z.25
G1Z-.5F.045
M5
G1Z.25F.055M4
M5
X30.Z30.M9
M1

[Thawk53]

Pyro,
Yes that should work. I think I would probably feed out at the correct pitch (.050) instead of .055. Make sure you leave the feedrate override at 100%.
Another thing, if your machine will accept M161, this will fix your feedrate at 100% no matter what the feedrate override is set on. M160 cancels M161.

Rick

[underthetire]

Should work fine. I agree withThawk53 on the M code and feed.

[pyropainter]

Thanks for the help. It will be a few days before I can try the program. I will let you know how it goes.
Barry

[pyropainter]

Thanks to everyone for the help. I was able to tap an M3 by .5 hole about .65 deep with a forming tap in aluminum. So far things are working great, thanks again.
Barry