Last thread pass ruining threads

[Cadencutsmetal]

I am trying to make 9/16-18-unf-2b internal threads, out of 316 stainless, i am having trouble w the back of my insert chipping out and chewing up my threads on the final pass, the threads look fine until taking to final size, have tried using micro threader but it seems to not be deep enough and will break the insert before final pass, I’m taking a .001 doc, 225rpm, and a federate of .0556, using fannuc controls
Current program lines are as follows
G76 p020060 Q0010
G76 x.563 z-.455 P0300 Q0010 f.0556

 

[bigjon61]

I am trying to make 9/16-18-unf-2b internal threads, out of 316 stainless, i am having trouble w the back of my insert chipping out and chewing up my threads on the final pass, the threads look fine until taking to final size, have tried using micro threader but it seems to not be deep enough and will break the insert before final pass, I’m taking a .001 doc, 225rpm, and a federate of .0556, using fannuc controls
Current program lines are as follows
G76 p020060 Q0010
G76 x.563 z-.455 P0300 Q0010 f.0556

Way way too slow. I make a part out of 304 and 316 that has 1/2NPT threads and got terrible tool life when running conservative spindle speeds. Crank that baby up to 1200-1500 rpm and make sure you have plenty of coolant to flush the chips out of the bore.

 

[colton_m]

Try 0.055556 for the feed.
All the controls I've ever used would take six decimal places in a threading cycle.
Sometimes you have to switch the F address to E for it to work.

 

[Mtndew]

Try 0.055556 for the feed.
All the controls I've ever used would take six decimal places in a threading cycle.
Sometimes you have to switch the F address to E for it to work.

While you are right, he's only cutting .455" of thread in Z so that small rounding error wouldn't make a difference.

 

[Mtndew]

Way way too slow.

I agree 1000%.

 

[sinha]

G76 p020060 Q0010

Insert finishing allowance (R word)

 

[Ox]

UNC

Q.001?
Shirley you should jack that up considerably!
(and add the R)


------------------

Think Snow Eh!
Ox

 

[Cadencutsmetal]

Way way too slow. I make a part out of 304 and 316 that has 1/2NPT threads and got terrible tool life when running conservative spindle speeds. Crank that baby up to 1200-1500 rpm and make sure you have plenty of coolant to flush the chips out of the bore.

Ramped speed up to 500 and lost issue atleast for the first part, I have a short run so I’m going to keep speeds climbing until I reach the 1200, thank you!

While you are right, he's only cutting .455" of thread in Z so that small rounding error wouldn't make a difference.

really less, .107 chamfer leading into the threads

 

[bigjon61]

Ramped speed up to 500 and lost issue atleast for the first part, I have a short run so I’m going to keep speeds climbing until I reach the 1200, thank you!

really less, .107 chamfer leading into the threads

If it were me, I'd keep increasing until results got worse. "Push it until it breaks then back it off 10%" -Boss

 

[Rogue_Machinist]

I can thread inconel 625 all day with a single insert. I think your G76 might be off a little bit. Maybe the first cut is too heavy.

 

[Thomas_Brown]

Sounds like a situation you're facing with those 9/16 18 UNF 2B threads, in 316 steel. I've encountered problems in the past. What usually works for me is adjusting the threading cycle specifically the G76 parameters. Making tweaks there can often lead to improvements. Also don't forget to pay attention to your tooling and coolant setup. It's crucial to ensure you're using the insert and providing coolant flow. Lastly you could try experimenting with a spindle speed but be careful not to put too much stress on the material.

 

[Cadencutsmetal]

Sounds like a situation you're facing with those 9/16 18 UNF 2B threads, in 316 steel. I've encountered problems in the past. What usually works for me is adjusting the threading cycle specifically the G76 parameters. Making tweaks there can often lead to improvements. Also don't forget to pay attention to your tooling and coolant setup. It's crucial to ensure you're using the insert and providing coolant flow. Lastly you could try experimenting with a spindle speed but be careful not to put too much stress on the material.

so my first cut is .001 radially, so 2 thou, and goes in 2 thou intervals until final pass which jumps from .551 to .563, that’s where all my problems have happened, threads look great until then, and then my insert chips out on that last pass. Not sure how to limit the doc on that final pass if even possible, I believe that’s where my biggest problem lies

 

[rjwalker1973]

so my first cut is .001 radially, so 2 thou, and goes in 2 thou intervals until final pass which jumps from .551 to .563, that’s where all my problems have happened, threads look great until then, and then my insert chips out on that last pass. Not sure how to limit the doc on that final pass if even possible, I believe that’s where my biggest problem lies

Increasing the depth of cut on the first cut will decrease the depth of cut on the last cut. I would bump that up. It may be work hardened by the time you get to the last cut from the shallow depth of cuts.

 

[sinha]

Is it 0.551 to 0.563, or 0.561 to 0.563?

 

[BT Fabrication]

so my first cut is .001 radially, so 2 thou, and goes in 2 thou intervals until final pass which jumps from .551 to .563, that’s where all my problems have happened, threads look great until then, and then my insert chips out on that last pass. Not sure how to limit the doc on that final pass if even possible, I believe that’s where my biggest problem lies

most guys doing threading will run it too slow, its actually always worse as it gets deeper in the thread and will end up pushing more material instead of cutting it. in threading, speed is your friend here and will usually fix the chip loading and chipping of inserts.

 

[Cadencutsmetal]

Is it 0.551 to 0.563, or 0.561 to 0.563?

100% is a jump from 551 to 563 for final pass, upped doc to .0025 and getting fatter cuts until I get to 551 but then still getting the jump in size which is chipping my insert, I have speeds up to 800 now, from originally 175, seeing improvement but still going thru an insert a part

 

[TeachMePlease]

100% is a jump from 551 to 563 for final pass, upped doc to .0025 and getting fatter cuts until I get to 551 but then still getting the jump in size which is chipping my insert, I have speeds up to 800 now, from originally 175, seeing improvement but still going thru an insert a part

Did you add the R word to your first G76 line, as suggested by two people previously? R is your finish cut allowance.

 

[rjwalker1973]

Did you add the R word to your first G76 line, as suggested by two people previously? R is your finish cut allowance.

exactly and if that still don't work change to a g92 and add the subsequent passes.

 

[Cadencutsmetal]

Did you add the R word to your first G76 line, as suggested by two people previously? R is your finish cut allowance.

Added r word, which gave me what I wanted, still having a little trouble but getting much closer to correct

 

[sinha]

Try reducing the minimum DOC (Q in the first block)
Same DOC in all passes is not recommended for a 60 deg insert. It should be gradually reduced.