I am using G76 to thread on my KIA 15 w/Yasnak control. It keeps ending with a .006 deep final pass. No matter what K, D, or final X I give it, it does a .006 final depth pass. I went to the extreme and got it threading with about .0004 per pass BUT it gets to .006 from the final depth and does 1 final .006 deep final pass. I am threading an M4x.7 thread, and just want to control the final pass. I have had no problems with other threading cycles, M2, M3, #4,#6,etc, but this one is kicking my tail. Keeps breaking my shaft on the last pass. Any ideas?

Material is 316 SS. RPM 1100.

Rapid to: X.167 Z.1
G76 Z-.775 X.110 K.022 D.007 A60 F.028

On my control fi i only use one line G6 it uses default values for finish pass DOC. Try using the two line version. Here's my G76 notes:

'*******TWO LINE FANUC G76 INSTRUCTIONS*********************

'NOTE: Use G0,G1 to position machine at start of thread(Z) and retract height(X) before G76 lines.
' Important: X position determines ID or OD threads


'EXAMPLE G76 LINE 1 FOR 1/2" ROD 20 TPI
'G76 P011060 Q50 R10
'first two digits after P number of finish cut passes
'second two digits after P number of leads to pull out/10, 10 is 1 lead
'third two digits after P is tool tip angle, tool will infeed at 1/2 this angle
'Q is minimum DOC cut in tenths, example 50= .0050 depth radius
'R is DOC finish passes in tenths
'S is optional spindle speed, spindle must be running with an earlier M3 M4 code

'EXAMPLE G76 line two 1/2" rod 20 TPI .5" long 1 thou taper (Z 0 at start of thread)
'G76 Z-.5 X.4567 P433 Q100 F.05 R.001
'Z is end of thread Z value
'X is final diameter of thread value; minor dia. on O.D., major dia. on I.D. (LH) threads
'P is thread height in tenths, 433 is .0433 high, generally COS(infeed angle)*1/thread pitch
'Q is depth of cut for first cut in tenths
'F is feed per thread, 1/LEAD for US
'R is for tapered threading difference in X from start to finish in Z

I don't believe Yasnac supports 2-line Fanuc cycles.

Don't know which control you have, but I believe on the LX3 setting #6206 sets the last depth of cut.

Thanks guys. The controller I have is the LXIII. We got this lathe in a buyout of another shop and I do a lot of prototype pins and shafts with it. Unfortunately we did not get very good manuals for it. So I am learning as I go.

You can download Yasnac manuals at:

http://www.yaskawa.com/site/dmcontrol.nsf/Productline.html!ReadForm&Start=1&Count=1000&Expand=20

I share your pain.
I too have a Kiaturn21 with LX3 control and very little documentation at my new job.
Dcoupar has it right on with the setting 6206 and only using the one line code.
Yaskawa.com has manuals but offer very little support if called about such an old control.
The control is Fanuc like but has some quirks to it.
Example- when using G71 and G70, unless your start point in X and the last X line in the profile are exactly the same value you will get an 095 alarm.
This drove me nuts until I figured it out.

Thanks for all the info guys. VERY helpful. Downloaded the manual and got my threading to work like a champ. Using the 1 line G76 is the way to go. Manual should also help in in linking the machine to the computer. Manual I got with the machine sucks as far as setting this up, downloaded manual seems to be far more informative. Thanks again.