[dingo0722]

Just wondering what would be recommended speeds and DOC for cutting a 1/4-20 thread, single point threading in 304. Right now we are running 750rpm at 0.008 DOC.

[SirDenisNayland]

I would be generally interested as well, as I have not had much luck single point threading in 304. Too little cut and you run the risk of work hardening, too hard a cut and your tool point chips.

I will say one thing though, your passes typically should be of a gradually decreasing depth of cut until you reach your desired finish diameter. That goes for any material as far as I am concerned.

[Shane1234]

i usually run around 1000 rpm, doc at .002 per side, and 3 spring passes. i can hold a corner for atleast 8 hours... this is a sandvik insert by the way, with coolant.

[dingo0722]

i usually run around 1000 rpm, doc at .002 per side, and 3 spring passes. i can hold a corner for atleast 8 hours... this is a sandvik insert by the way, with coolant.

so you are running .004 DOC in diameter. How do you program in for spring passes? Do you just add the code manually after the threading CAN cycle?

[Shane1234]

so you are running .004 DOC in diameter. How do you program in for spring passes? Do you just add the code manually after the threading CAN cycle?

spring passes are in the can cycle my friend. :rainfro:

lets start class, as i know how fun it was to teach myself this crap, haha....
(group)

g76 p040060 q0020 r.001
g76 x.? z-? p0400 q0100 r.000 f.05

my machine doesn't use the 2nd line Q, it bases it off the second line P, so no need for the second line q. your machine might, so i pulled an example of it. also, my machine requires decimal in the r value, but not the q & p, so it may vary for you. q0020 is .002 thousandths, but my machine does g76 canned cycle in radius, not in diameter, so the .004 i want in diameter has to be programmed in radius.

your spring passes is the first 2 numbers in the first line p. p"04"0060 . 04 is the amount of spring passes. most of the time you wont need to change the 60 on the end, unless you start programming acme threads or specialty threads.....


First line of G76 the P is: 1st pair is number of free passes (a.k.a. spring passes) at final depth
2nd pair is number of "leads" to exit at the Z axis end of stroke ex. 32 means 3.2 turns of pullout, starts pulling X axis out at (.125 x 3.2=.4) from end Z position, offering a stronger thread. Good for high strength studs
3rd pair is the included angle of the thread, needed to work the insert in in the "compound angle"

the Q is: "clamp value", meaning the smallest increment the infeed goes to in the penultimate pass. Working in conjunction with the second line's Q value, this Q value helps determine the total number of strokes it will takes to complete the cycle. Bigger 1st Q, fewer strokes, smaller means more finite stepping down to size. Normally, I never have that R be larger than the Q.

The R is: final pass depth before the "free passes" of the first two digits of the 1st G76's P code.

The SECOND G76:

X is the final "root" or "minor" diameter of the thread
Z is your length from the Z zero point
P is the incremental ("on a side") height of the thread
Q is the incremental depth of the first pass
R is (optional) incremental taper of the thread. Use this when making a tapared (pipe) thread or for correcting slight tapers in a long, unsupported thread.
F is the feed rate for the pitch (lead) of the thread. Your 20 pitch example: 1 divided by 20 = .05