Any help on this one? having diffuculty with the G76 cycle. Are there any "simple" ways to calculate for X, P, R, etc????? I'm new to this whole tapered thread thing and evidently, so is everyone that works above me - I"M FRUSTRATED!!!!!!!! Any info would be greatly appreciated.

Not much info on the bspt in the machinist hand book
but this is what i found.
major dia 2.347
minor dia 2.2306
thread height .0582
lenth of thread 1.8624
taper 1.7899 deg.
This is the g76 program for a fanuc 21t control
if you have a different control let me know.
Cut taper first

G0 X2.397 Z.2254( threading tool start)
G76 P020160 Q0050 R.001
G76 X2.119 Z-1.8624 R-.0652 P0558 Q0100F.09091

To find thread height mutpily lead x .61413 ( this formula will get you close it does not always agree with the machinist handbook)
example lead .09091 x.61413=.0558 x 2 = .1116
minor dia. 2.2306 -.1116 = 2.119 ( final x position)

The R is the differance in height of the thread angle from the start of the theading tool to the end of the thread example, thread lenth 1.8624 + tool start lenth .2254 = 2.0878

2.0878 trig (1.7899 angle of taper)= .0652


Have fun
tim

Thanks. I'll give it a shot and let ya know.

Thanks. I'll give it a shot and let ya know.

Or try this I found this on line a few years back it works great if you have the Fanuc w/macro capabilities

In main program:
G65 P9000 U0. W0. A.375 R5. E10. Z-.5 V18. F10.

O9000 (PIPE THREADS)
(U IS X LOCATION)
(W IS Y LOCATION)
(A=STARTING RADIUS)
(R=NUMBER OF MOVES PER CIRCLE)
(Z=DEPTH)
(E=NUMBER OF PASSES [thickness / pitch])
(V=THREADS PER INCH)
(F=FEED)
#3=0.0
#10=360 / #18
#109=#10
#110=1 / #22
#111=0.0625 / #22
#3=#18
G00 X#21 Y#23
G01 Z#26 F#9
#19=#1 + #21
G01 X#19 Y#23 F#9
N2 #26=#26 + #110 / #109
#24=COS[ #3 ] * #1
#25=SIN[ #3 ] * #1
#24=#24 + #21
#25=#25 + #23
G01 X#24 Y#25 Z#26 F#9
#3=#3 + #18
#1=#1 + #111 / #109
IF [ #3 LE 360.00000 * #8 ] GOTO2
G01 X#21 Y#23 F10.
G00 Z1. M09
M99

Bluesman

that will work awesome for me. every few days im doing a new program and about 70-80% of them are pipe threads. thanks a ton. my life is getting easier! :cheers:

How do you use g76 on standarts threads on fanuc 21t. exaple would be great. thanks

How do you use g76 on standarts threads on fanuc 21t. exaple would be great. thanks


LOOK AT TYHE FIRST POSTING IN THIS THREAD. BUT ALSO THE PARAMETERS TO CONTROL THE CYCLE ON A 21I(T) ARE AS FOLLOWS

5140 DEPTH OF CUT PER PASS
5141 FINISH ALLOWONCE(DEPTH OF CUT FOR FINAL 3 PASSES)
5142 REPAET PASSES ( REPETITIVE PASSES TOP CLEAN OUT ANY TOOL DEFLECTION AND GET A GOOD CLEAN THREAD FORM)
5143 TOOL NOSE ANGLE


THESE PARAMETERS ARE CRITICAL FOR CUTTING NICE CLEAN THREADS

BLUESMAN

I use G92 for all standard threads as you can choose the next cut depth as you wish; not determind by the paramteres,

I use G76 on large pitch or multiple start threads as there are too many passes to warrent using G92

Don't forget the I value (I-.?) for external and (I.?) for internal
But of course everyone has there preference, the advantage of G92 is you can restart a your thread from half way through the cycle instead of the beginning saving time cutting mid air passes.

Once again is just personal preference.

This is a great site!!!