Single point threading nitronic 60

[Joeandrus]

I’m machining some hex coupling nuts with an id thread of 7/8-9 UNC 2A 1.5” depth. I can’t get the thread insert to last for more than maybe 2-3 pieces. The drilled hole is at 1.650 depth and I have two thread cycles so I can clear out shavings that get stuck at the back. I’ve tried different speeds and depth of cut but every time the tip chips off of the thread insert. Thread cycle is running G76 P010060 Q30 R0.
G76 X.875 Z-1.56 P601 Q60 R0. F.1111
Thread insert is a Vardex VTX.

 

[Milland]

How rigid is your setup? Is the insert on center, or a touch above? If on center, might be worth shimming it 5 or 10 thou higher to prevent "digging in".

 

[Joeandrus]

How rigid is your setup? Is the insert on center, or a touch above? If on center, might be worth shimming it 5 or 10 thou higher to prevent "digging in".

Setup is pretty rigid I’m using an iscar sir 0625 p16 lay down thread bar. It’s on center as far as I can check.

 

[Milland]

If you feel like experimenting, raise it up a bit. Can't guarantee anything, but it's worth a shot. Are you getting good coolant flow into the hole, and is it to spec?

 

[Joeandrus]

If you feel like experimenting, raise it up a bit. Can't guarantee anything, but it's worth a shot. Are you getting good coolant flow into the hole, and is it to spec?

Coolant is blowing right into the hole until maybe the last .150. What do you mean by raise it up a bit? I can try it when I go back in tomorrow.

 

[Milland]

Raise up the insert, presumably by shimming the bar in the tool block (or whatever method you use). If the tool edge is on center in a boring op, if there's deflection the load on the tool edge increases due to geometry. If you raise the tool a bit (.005/.010) it helps prevent this load increase while not disrupting the cutting action too much (unless you're facing to center, which tends not to happen with a threading insert!).

If it's a round bar in a tool block bore, an offset bushing may be needed. Or if the bar can be rotated a tiny bit, that can be tried.

 

[gcodeguy]

Been quite awhile since I've run any of this type material. Quick search shows it has a high work hardening rate. You may want to give an R-value in the first block. (And I don't mean R.0005 ) I'm going to guess your RPM is below 1000. Are you having a chatter problem? That is pretty much the only time I use a 60 compound infeed since it only cuts on one side of the insert. Have you tried a 29 or 55 compound infeed?

Is the VTX the grade Vardex suggested for this material? Maybe the VRX or VM7 would be a better choice? We have a few Vardex inserts, but I must admit they don't get used often.

I hate small internal threads. We just finished a 5/8-18 UNF in 316 SS casting. Blind hole. Machined the same way you are. Finish bore, re-drill, rough thread, re-drill, finish thread, re-drill, re-bore, re-thread. What a PITA. Has run many times before, but had to drop DOC on first pass and RPM this time. Like you we were only getting 2-3 parts per corner.

Don't you just love it when a program runs fine the first time (or a few times), then like crap another time?

 

[guythatbrews]

7/8-9 1.5 deep sounds awful in about any material let alone this stuff.

Are you using a coolant through boring bar? That will help. Of course high pressure coolant if you've got it.

So threading into a blind hole and parting off? Any way part off and thread the through hole? You barely have any room at the bottom of the hole. If chips are packing that is death to the tool and certain rapid failure.

Use a full profile insert so the tip truncation is a big as possible. Make sure the minor diameter is as big as you can get it.

Any live tools? Can you threadmill it? Even if you turn the blank and move to a milling machine to threadmill you may be money ahead.

Good luck!

 

[MaxPrairie]

What is the thread pitch range for the insert you are using? How do the threads look on a fresh insert and how does it sound while cutting? I would think you would be able to hear that corner popping off.

 

[angelw]

I’m machining some hex coupling nuts with an id thread of 7/8-9 UNC 2A 1.5” depth. I can’t get the thread insert to last for more than maybe 2-3 pieces. The drilled hole is at 1.650 depth and I have two thread cycles so I can clear out shavings that get stuck at the back. I’ve tried different speeds and depth of cut but every time the tip chips off of the thread insert. Thread cycle is running G76 P010060 Q30 R0.
G76 X.875 Z-1.56 P601 Q60 R0. F.1111
Thread insert is a Vardex VTX.

Your program, with a first pass DOC of 0.006" and a minimum DOC set at 0.003", will cut all threading passes except the very first, at 0.003". With that material and that meager DOC, the insert will be doing more rubbing than cutting. Even when cutting, the number of threading passes per part equates to a lot of work by the insert per part, so, little wonder you're not getting many parts per insert.
Regards,

Bill