Problem- g71 okuma help

[Peerless]

Im using an okuma lathe with an osp700l controller and Im trying to write a g71 threading program and in cncezpro it seems to cut way too deep and crash. I am following the okuma sheet for writing the line and I am getting no where. Any help would be, well, helpful. Trying to make a 2-56 thread, Major Dia- 0.0854 Minor Dia- 0.0813 code:

N10 T0100
N20 G50 S2500
N30 G00 G97 S125 M03 Z1.0 T0101
N40 X0.300
N45 Z0.300
N50 G71 X0.0813 Z-0.250 B60 D0.005 F1 J56 H0.0082 M08
N60 G00 X25 M09
N70 Z25
N80 M01

I am also using peter smids cnc techniques, but so far it just makes things a bit more confusing. Thanks again

[g-codeguy]

We have one Okuma (think it is the same control), but the other programmer is the one who normally programs it. However I have done a couple programs for it over the years. Not at work, so I can't get to a manual to check your code.

Several things:

1) Don't recall ever using J for the lead.
2) Remember an M-code at the end, but it sure wasn't an M8. M32 maybe?
3) X.3 is much larger than necessary. Try X.12
4) S125 is extremely slow. Run wide open at that diameter and pitch.
5) What is the F1?
6) Is there a reason for your rapid moves being in an "L"?

Have NEVER threaded something that small. Definitely need to keep the cuts very light. Personally I don't hold out much hope for your success. I've seen cut-off pips bigger than that.

Sorry I couldn't be of more help. I will check out the code Monday if you haven't solved the problem by then.

[broby]

Wow, have never tried cutting such a small thread!
Obviously your tooling setup will have to be absolutely smack on centre height otherwise forget it!
As for running really fast, be carefull as you will get pitch errors the faster you go. There is a formular that you can use to calculate the distance required for the starting and ending distance, but that info is at work...
G-Codeguy, the F1 J56 is the way that you can accurately set the pitch for odd threads. In this program, the feed will be calculated as being 1/56th of an inch or 0.017857"
When cutting TPI it is much easier to use I and J than to specify the thread pitch. Also the Okuma control does not allow anything other than a whole number for the J value, so to program a 11.5TPI thread you need to use I2 J23 (23 threads per 2 inches)
I would think that you also need a finish cut allowance in your threading cycle using a value "U", in your thread, being so small I would guess maybe U0.0005" ?
Your thread height value seems a bit large as there is only 0.0041" (on diameter) between your Major and Minor Diameters. Have not got any thread tables here(home) to check this, I would suggest a value around H0.003, Changing this value will allow you to control the depth of cut on the first pass.
Your depth of cut at D0.005 is also very large considering the above diameters of the thread. This needs to be reduced to around the D0.001 value.
Remove the M08 at the end of the line.
You need to also specify the infeed pattern that you will be wanting to cut the thread with. This is done with a combination of 2 different M codes.
Hope I remember these correctly... it has been a while since I have used them much.
M32 Infeed down the left flank of the thread
M33 Zig Zag infeed pattern
M34 Infeed down the right flank.
M73 Infeed pattern 1, This is a reducing depth of cut cycle, I do not recall using much.
M74 Pattern 2. Mainly used this cycle. Infeed is made by D(on Diameter) in each pass until "H-U (W)" is reached, after that, finishing cut is made with infeed amount of U. if no U value specified, then no finish cut is performed.
M75 Pattern 3 (horrible one, takes forever)

Hope some of this information helps.
Regards
Brian.

[Peerless]

thanks a lot for the information! I had some numbers wrong in my original post, the thread height is a lot bigger. I modified the the line and its working now. I dont have access to it right now.

Also, my g00s start in an L because there is a really big tailstock. It would prob be alright but I do what Im told to do.

Thanks again