Post By PixMan
G76 thread cycle
I am cutting an internal thread using a G76 thread cycle. 1.062 dia x 16TPI. My threading tool drags on the retraction back to the start point. Any one know which parameter needs to be changed to allow for more retraction to clear the thread. Fanuc 18I TB control.
Increase the depth of thread.
P word - 2nd line.
G76 thread cycle
If you mean that the tool drags on the ID as it comes out, change the point where you start to a smaller diameter.
I have some examples for this on my website: www.doccnc.com
The typical Canned Cycles to make programming a lot easier:
G71 does turning-boring with very little info.
G76 cuts a thread, straight or tapered, also with very short, basic info.
Example: G76 Threading Cycle in 2 line format for OT and later controls.
2" diameter, 20 Threads per Inch, Mild Steel.
N1 G50 S1500*
N3 G97 S700 M3*(Speed for threading, always in RPM)
N4 G0 X2.2 Z.2 M8*(Rapid to above part, .2" from face)
N5 G76 P021060 Q20 R5*(The first 2 digits in P represent the amount of finish passes, the next 2 are the pullout distance at the end of the threading motion, expressed in tenths of revolutions, the 60 is the angle of the tool)
N6 G76 X1.94 Z-1.0 P300(total thread depth) Q150(depth of first cut) F.05*
R if needed is the amount of taper over total distance in thread motion.
The P value is figured by taking the F-value times the constant of .6, once figured you also have the X value.( The actual value is P times .62 but its safer to use .6 as a constant and the correct the size by using an offset)
N7 G0 X6.0 Z6.0 M9*
Good luck: Heinz.
You didn't state whether your machine uses the two-line or one-line format for the G76 cycle.
Assuming you use the two-line format, give yourself a little more clearance on the START POSITION of X.
I'll assume that because you're making a 16TPI thread to a 1.062 diameter that you're starting with about a 1" bore. Where's your starting point of X? I'd probably be safe with something like .980" or .970, but even if you're closer to 1" you might need to adjust because...
The cycle effectively "calculates backward". For an internal thread, it takes the value of the "P" in the second line, doubles it and and subtracts it from the final dimension for X that's also in that 2nd G76 line. Your first pass is that calculated diameter minus 2x the value of the 2nd line "Q". The retraction is to the final diameter + 2x the value of P in the 2nd line.
As Ox said, increase that P. However, be sure it adds up to still a bigger diameter than your FIRST POSITION of X. For example: If the final diameter (1.062) minus 2x the P (say 0300) = 1.002 but your first position is 1.010, things can get screwy. Start further away so there's plenty of room for the calculating done by the cycle.
Am I the only one here that uses the G92 thread program? I like it a lot better because you have better control of DOC and chip load.
G92 X1.01 Z-.5? F.0625
G0 X.96 Z.25
Never used it.
What chip load/DOC issues doo you have with 76?
Other than the [non] alternating flanks part - I see nothing much to be gained from 76. ???
76 will keep chip load a LOT closer than you just did. (n't)
Did yours infeed on a 60? Or straight plunge? I don't see any callout for infeed angle. ???
I'm thinkin' that you don't fully understand 76. ???
You need a chart that Fanuc doesn't provide (that I know of) to really make sence of it. That chart can be found in Kennametal Cat #1010 page 683. That chart should be hung on the wall by any normal programming desk!
(Mine is still only in the Cat. So I kant post a copy of it.)
Think Snow Eh!
Last edited by Ox; 04-28-2010 at 04:12 PM.
No, I use it too, except only for special purposes:
On the Haas, I use G76 for the main body of the threading and use G92 for "chasing" the thread. Basically to comb off the small burrs ( after an OD chase)
On the Fanuck, the G92 does NOT follow the G76's path, so I'm stuck with G76 for the chasing cycle as well. BUT! When some idiot engineer specifies no thread chamfer OR a 30deg chamfer on the front of the part, I use G92 all the way because it allows precise depth control which is very helpful in chip/chatter removal.
Originally Posted by Ox
Yes, G76 will keep better chipload control, but with G92 you can do some fancy things as I've mentioned before.
Another example would be when you have something thin walled and you get chatter on the threads. With G92 you can take a pass or two at the X-min diameter, then move up .0002 or .0003 and take a few more.
This always removes burrs and chatter.
Seems a little easier than monkeying with the G76 cycle.
Try it, my example was a quicky, easy to change loads and passes, only drawback is you can't easily do 60 deg. angle infeed but we have software that will change Z start point on each pass get the 60 deg., but I usually feed in straight as I have found I get better tool life that way. And yes I do FULLY understand G76, both single and double line and I still prefer G92 most of the time.
Originally Posted by Ox
hi, want to know about G76 Threading cycle on CNC Fanuc controls read cnc blog post about G76 threading cycle CNC Canned Cycle G76 Threading Cycle for Fanuc CNC Machine Control
hi, this throws more light on G76 threading cycle. And how to set the diameter for internal and external threading G76 thread cycle Fanuc Tips for Setting Thread Diameter for Internal and External Threading
I would use a smaller boring bar!
But I must say Doc Seymore and Ox give very good solutions as well
I see that you pulled up an old thread...
Let me update this a bit.
I took a pic of that page a while ago and posted on another thread.
Think Snow Eh!