Hardinge threading code

[Pontiff51]

Hi everyone. I'm trying to cut a ID thread in our CNC lathe.
It is a Talent 6/45-SV with a Fanuc SV controller.
The machinist who just quit was the only one with experience on this mach. I understand that this mach. takes 2 (two) G76 lines of code to cut a thread. We have asked the mfg. for the CD with the manual a couple of times, but we still havn't got one yet. If anyone can help out with the format and explaination of the coding, you would have a friend for life. Thanks.

[carlos1970]

actually
it can use one g76 line
i use a haas sl20 machine
i made a mistake in downlaoding a haas program into the talent and
was editing the g76 line and forgot to add the extra g76

guess what the talent worked with out the first g76 line
worked with g76 x2.0z-2.0 d.02 f.0555

the first g76 line identifies the thread angle and such info
the 2nd line tells the machine the z and x and feed and height of thread
bear with the fanuc style programing its not difficult

[Karl_T]

The key to ID vs. OD is your position when G76 is callled. See my cheat sheet.

'*******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
--

[g-codeguy]

The only thing I can add to Karl's excellent explaination is that the X_Z_ value is the ENDING position for both axis. That means if you are threading an I.D. pipe thread the R value will be plus. For an O.D. pipe thread it will be minus.

On our Okuma it is just the opposite. X is the value at the starting point.

Oh yeah. X starting positon is common sense. It is the dimension the tool retracts to after making a threading pass. You wouldn't try to thread a 1/2-13 O.D. thread with a starting position of X.46 would you?