Thread: High temp alloy pipe threading

I need some suggestions on single pointing 1/2"-14 NPT threads on high temp alloys...specifically Inconel 718. I've tried Sandvik 1020 with standard chipbreaker and their F geometry (ground with sharper edges), Vardex (VM7, VKX, and VTX), and Carboloy along with extensive help from their sales and threading specialists (they are baffled).

I don't have any problems with any other turning operations, other thread types, or drilling (all carbide)...but these NPT threads suck.

I've run a pretty large spectrum of SFM and # of passes, different infeed styles (flank, modified flank, ziz-zag, etc...), even rough threading and finish threading with two different inserts (just barely works and then only with good operators...unfortunately, gotta program for the lowest common denominator).

The most I've been able to get is five parts/edge. Any suggestions or tricks?

175sfpm
.005 doc

Pi, don't you mean 172sfpm?

Actually, another approach is to rough the thread with a truncated insert (flatted end) in zigzag style cut (alternate sides of the flank). It would take two tools to accomplish this, and getting them both in register could be a bit of a trick. But at least the finish tool might last a while longer than if it cuts the entire thread.

Bradley

I think Hu has the right idea, even though it may take a little DWI. U can abuse the roughing tool for some time and the finish tool should last 20-30 parts. My thing was a 1.0625-12 UNJ thread, 450 pieces. The only way I was able to save my sanity is using two tools. Program to full depth on the 1st one, it will only take 2-3 parts and it will be well above size. Use the finish tool and take 4-5 passes to get to finish size and spring 3-4 more times there.

OD por ID thread?

OD or ID thread?

I've already tried the higher SFMs...up to 200 and 11-12 passes (as suggested by Vardex). That comes out to about .005 DOC average but I was allowing the thread cycle to progressively cut shallower depths. This is strain hardened stock (about 30-32 hrc vs. 20-22 hrc for annealed). I'll have to try programming .005 all the way down. Flank infeed...modified or what pi?

I also already tried (see original post) the rough and finish thread that Hu and seymor suggested. Didn't get consistent results with that and also cannot always rely on my better operators being on the machine. A good portion of the operators are button pushers...unable to understand what to do when finish problems show up on the thread flanks due to the two different tools.
I don't have any problems with UN threads...UNJ would be slightly easier due to larger root radius than UN.
This is OD and ID.

Bradley
Well, Inco has a way of making even the best of us cry. Been there.
See if you got Valenite VC929 grade inserts, I've had some decent luck with them on smaller (1/2") thread. I am not sure what is the size you're cutting, but if it is pretty large and coarse the problem is that too much of the tool is buried in the part.
I have not tried it yet, but one of my customer used to make tons of 1-8 threads on 625 annealed though. He had the same problem (obviously), and what they ended up doing is manually programming leading/trailing edge cutting using G76. This way they were able to control the DOC on each individual pass independently. I know it is a PIA and even worse on NPT but you may want to give it a try.
Also, you said OD and ID. What is your wall thickness? Can some of your problems caused by chatter? On the OD thread it may help if you plug the ID with a rubber plug.

i have never had luck with zigzag threading. the tips of thread inserts are so weak that creating wear on both sides substantially decreases tool life. inconel like low rpm, high feed, low doc and uncoated aluminum grade inserts.

My theory is that zig-zag threading will decrease the overall pressure required to force the tool into the cut (by half), thus gaining an advantage on work-hardening materials. It should also improve chip flow (less of a channel shape to the chip). On slender workpieces, the tendency to chatter and or deflect is much reduced. I learned this on manual lathe, so it must be correct

I cannot see that favoring one side of the insert over the other has any logical benefit.

by only weakening 1 edge the other provides strong support

Slow...175, or even 100 sfm would be appropriate.
Use G92. Threading Inconel 718 is one of the instances where it really is worth the effort to wtite in the extra code.
Consider using a rougher to absorb the wear...if you've got the space for another tool.
Make your Z clearance plane big enough that you can index inserts in mid program, with feed hold & spindle off, and resume threading.

Or you can try something like this:

G50 S900
G00 G97 T303 S500 M03
G00 X1.066 Z0.05 M08
G76 D0.01 A60 F0.0833 X0.9616 K0.0476 Z-0.57 <-thread
G80
T303 <-- re-call same tool or a finish tool
G00 X1.066 Z0.05 M08
G97 S500 M03
G92 X0.9636 Z-0.57 F0.0833 <-spring to the finish dia
X0.9626
X0.9616
X0.9616
X0.9620 <- helps with burr
G80

Obviously, if you call a different tool for the spring pass you may want to move to a clear position first.

Thanks for the replies...BUT, here's the thing. Standard screw threads are not a problem for me (UN, UNJ, metric, Whitworth, etc...) but these NPT's are. If you actually have experience with NPT (OD & ID 1/2" preferred) threads in 718, X-750, 625 or Hastelloy C-276 I'd like to hear how you do it.

I can run at fairly decent production rates with other threads in some of the other high temp alloys. Not all Inconel alloys are alike...Inconel 600 and 718 are like worlds apart in machinability...just like UN threads and NPT threads. Mix 718 and NPT together and it just gets worse.

I've been cutting these threads for about eight years and have tried things from time to time. Pretty much accepted what we were getting but figured it was time to make things better because of an increase in demand for the material.

Bradley, it really sounds like you've got an operator problem, rather than a machining one. If hiring someone experienced to run these NPT's isn't an option...how about making some thread gages (+.01 OD,-.01 ID), and tossing in a program stop after a rougher to help the button pushers decide when to change inserts?
You say you're not having any problems with other threading and turning in 718, which kinda surprises me. May I ask what inserts you're using, what SFM, and how many parts per edge on those operations?

I'm using mainly Sandvik SS grade inserts due to most of my work in SS (1025 MF for finish @ 200 sfm, 2025 MR or MM for rough @ 140sfm...faster for some of the other easier high temp alloys). I've messed around with inserts geared to the high temp alloys for turning...Sandvik S05F & 1005...they were better but didn't blow the SS grades away enough to make a switch. Also tried uncoated (H10 & H13) but they failed miserably. I will try some different chipbreakers though (Sandvik AL H10).

The alloys are usually short runs (5-10 pcs). It's not worth the insert switch and ensuring that the right insert gets used by the button pusher operator. Every once in awhile that 5-10 pc order may be a 100 pc order...that's when it becomes painful with the NPT threads. I can consistently run 20-25 pcs/edge on a 12 UN thread at 130 sfm. I'm lucky if I get 5 off a 1/2"-14 NPT...whether at 190 sfm or at 80 sfm and everywhere in between. I've checked center height, insert shim angle (tried two different angles), holder screws...etc. Also tried different coolants and machines to see if they made a difference. Everything I try is on a production schedule though so I don't have a whole lot of time to fool around...gotta get the next job going.

Bradley

I am a one man show,parts are normally 10 - 200 piece orders so doing it is not a problem, but unless the material is AL or brass, I always check the thread on the machine before removing it. I do turn inco often enough, and know that there is no way you can do too many of them without offset adjustment.
My threads are mostly J threads and I use Tri-rolls, but even then there is a GO gage to see if the part can come off the machine.
May be a PIA, but at these mat. costs well worth the effort.

Get a Kennametal (800-446-7738) catalog & look at KC5510 & KC5525 grades for hi-temp alloys & run according to their spec's. These are really good grades for that type of mat'l. & works well. If you are on a manual lathe everything changes due to rigidity. go with KC730 & you should be ok.

Run a part Inco 901 with 5/8-18 ID thread. Used the Vardex VKX, but only lasted 2-3 parts per tip. Recently started using KC5510, and now gets 1-2 parts per tip. This material is Rc 40-45.

Have been using 50 SFM and .005 DOC with .002 DOC on last two passes. Ordered a Johnson gage so operators would know how much to move offset, but still keep oversizing threads. There doesn't seem to be consistency between material left and offset adjustment.

Can anyone suggest different DOC / SFM parameters?

I cut quite a lot of npt threads on super duplex which is also pretty nasty stuff to cut.

Sorry if this is a stupid question but are you turning the taper on the pipe prior to threading, or are you just threading into depth?

My experience with NPT inserts in tough materials is that the sharp point is very fragile. When the tip fails it usually does so on the first pass. Try increasing the X start point slightly to reduce the amount of material cut on the first pass.

In SD my limit with sandvik 1020 is about 50m/min which is somewhere around your 175sfmm figure, but I'd up the number of passes. For a 14 NPT I'm usually up around 20-25, otherwise the tip fails very quickly like you are experiencing.

Gregor