trouble cutting a 8 TPI thread in SS304 - engine lathe

[rogertoolmaker]

Animal fats are the most tenacious of the oils. I've used lard in oil. Straight raw bacon grease may even be better. Never tried it! If the parts are to be cleaned, use a detergent.

Roger

 

[draganm]

Just an observation from an engineering point of view. The top of that holder seems to have no reason for sticking out so far. The downward force from cutting will try to rotate the insert away from that excessive overhang, probably opening the gap which the chip is getting caught in.

Another thing that is not helping you is the 36 pitch part of the insert. It's way more pointed than it needs to be. The tip will break down for a nothing.

I abandoned that holder and that insert last Thursday. I'm using an NT3 Top-load like eKretz talks about. It's rated for
6-20 tpi external
5-12 internal.
It's a big insert, and according to the handbook, i can't tolerate an overly large truncation at the root anyway. Max flat width .009", min. .005"

I'm sure there's better tools out there too, but i had this holder in my inventory and it's just this one assembly and hopefully never again.

So got the pipe today, 4 footer. More problems. My lathe is a 60" bed, should be well capable of a 48" turn, and it is, except for the Damn DRO. Looks like someone put a 53" scale on it, probably 50" of travel. Scale is bottoming out, not good
Now i have to check with the engineer, see if they're willing to accept a 45.0 or 46.0" long part. I have feeling there's more problems to come too.

Starting to think about sending this out and making it someone else's problem. I'm getting behind and too many days now fighting this dam pipe

 

[guythatbrews]

I abandoned that holder and that insert last Thursday. I'm using an NT3 Top-load like eKretz talks about. It's rated for
6-20 tpi external
5-12 internal.
It's a big insert, and according to the handbook, i can't tolerate an overly large truncation at the root anyway. Max flat width .009", min. .005"

I didn't catch this was a NPSM thread. If you really have to adhere to Crest and root truncation you probably need to get an insert intended to cut 8 TPI NPSM threads. The multi pitch un stuff won't do it.

 

[HappyWyo]

You already know it is harder to cut a 8 tpi thread than to cut a fine thread.
We learned a long time ago not to try cutting threads without lard. The larger the thread the more important it is.
I built a lard container that is attached to my taper attachment with a brush holder hanging from the side of it so it is handy at all times. We buy it by the bucket from Walmart. Also If you turn to fast it will create heat and your threads won't look nice. We wasted a lot of steal learning to slow down. It sounds like you are slowing down already. Our inserts last an unbelievable long time.
Good luck. Practice makes perfect.

 

[eKretz]

You already know it is harder to cut a 8 tpi thread than to cut a fine thread.
We learned a long time ago not to try cutting threads without lard. The larger the thread the more important it is.
I built a lard container that is attached to my taper attachment with a brush holder hanging from the side of it so it is handy at all times. We buy it by the bucket from Walmart. Also If you turn to fast it will create heat and your threads won't look nice. We wasted a lot of steal learning to slow down. It sounds like you are slowing down already. Our inserts last an unbelievable long time.
Good luck. Practice makes perfect.

Hmm, that's the opposite of my experience when using carbide...speed is very helpful indeed to get a good finish. Not so much with HSS though.

 

[HappyWyo]

Hmm, that's the opposite of my experience when using carbide...speed is very helpful indeed to get a good finish. Not so much with HSS though.

That's true when turning a shaft down. The faster the better. I especially like speed for ceramic. But for threads the heat is a killer. At least that's the way it works in our shop.

 

[eKretz]

That's true when turning a shaft down. The faster the better. I especially like speed for ceramic. But for threads the heat is a killer. At least that's the way it works in our shop.

Might be tooling specific. I like to thread right around 250-300 SFM when using the NTU inserts I linked above. They almost always produce smooth shiny threads at that speed. Good chip control too.

 

[LKeithR]

I've used "Top Notch" style threading and grooving inserts for years and I don't remember ever having
a problem like that. Haven't done a ton of SS but I've done some and if there's a problem it's usually the
material itself. Can you grab a piece of "known" material and see how it works...

Kennametal Top-Notch Grooving and Threading Inserts

 

[draganm]

I didn't catch this was a NPSM thread. If you really have to adhere to Crest and root truncation

I just noticed the .005-.009" truncated flats specs i referenced are actually for tapered thread.
For NPS, they don't actually list it, just state that major diameter external and minor diameter internal are truncated/calculated to avoid interference at crest and root. The only reason we picked this thread is it maximizes the material available for both the thread and ID bore in schedule 80 pipe (.325 wall thickness), without having to go to a massive schedule 160 pipe and losing too much area on the ID.
Today i also had the hopeful idea of doing the end-caps internal thread on the CNC mill interpolating with a threading tool. Maritool offers a part number 1310-.740-1 that can do 6-32 tpi. range, not ideal, but it looks like it could work. Anyone ever interpolate a thread this large on 304SS? I never have

Coating: TiAlN
Crest Width: 0.0029
Cutting Diameter: .740
Material: Solid Micrograin Carbide
Neck Diameter: .490
Neck Length: 2.0
Number of Flutes: 6
Shank Size: .750
Tool Diameter Range: minimum internal -1.0", Thread range 6-32 Threads Per Inch
Total Length: 5.0

 

[Kingbob]

"ASTM A312 is an American Standard specification which covers seamless, straight-seam welded, and heavily cold worked welded austenitic stainless steel pipe intended for high-temperature and general corrosive service. The most common grades are 304/304L Stainless Steel and 316/316L Stainless Steel ."

Well there's yer problem. That big chunk of welded on stainless in the first picture is either a chunk of the weld seem or just a big hard spot from being cold worked.
Seems you played your self sir.
Just kidding but we do have a policy round here about no threaded parts from welded pipe for a reason.

 

[draganm]

"ASTM A312 is an American Standard specification which covers seamless, straight-seam welded, and heavily cold worked welded austenitic stainless steel pipe intended for high-temperature and general corrosive service. The most common grades are 304/304L Stainless Steel and 316/316L Stainless Steel ."

Well there's yer problem. That big chunk of welded on stainless in the first picture is either a chunk of the weld seem or just a big hard spot from being cold worked.
Seems you played your self sir.
Just kidding but we do have a policy round here about no threaded parts from welded pipe for a reason.

LOL, yeah that was the test piece, obviously welded. The actual 46" piece is seamless, but still falls under the shite-material description above. IT's gummy, no 2 ways about it.

We'll see, it's finally in the machine now, cleaning up OD + precision bore on ID both ends. Then when that's done, the dreaded 8tpi thread. Trying to look on the bright side, at least i can still lift a 60 pound piece of stock into the lathe.

 

[guythatbrews]

I just noticed the .005-.009" truncated flats specs i referenced are actually for tapered thread.
For NPS, they don't actually list it, just state that major diameter external and minor diameter internal are truncated/calculated to avoid interference at crest and root. The only reason we picked this thread is it maximizes the material available for both the thread and ID bore in schedule 80 pipe (.325 wall thickness), without having to go to a massive schedule 160 pipe and losing too much area on the ID.
Today i also had the hopeful idea of doing the end-caps internal thread on the CNC mill interpolating with a threading tool. Maritool offers a part number 1310-.740-1 that can do 6-32 tpi. range, not ideal, but it looks like it could work. Anyone ever interpolate a thread this large on 304SS? I never have

Coating: TiAlN
Crest Width: 0.0029
Cutting Diameter: .740
Material: Solid Micrograin Carbide
Neck Diameter: .490
Neck Length: 2.0
Number of Flutes: 6
Shank Size: .750
Tool Diameter Range: minimum internal -1.0", Thread range 6-32 Threads Per Inch
Total Length: 5.0

I read the bit about the truncation in Machinery's handbook and just accepting the truncation as it falls out with normal straight pipe taps and dies. Not very definitive is it?

I think thread milling will work great but don't think you are helping yourself using a single row cutter that will cut 32 TPI. That sharp point will break down easier, especially with the material you have to remove. I would use a multi-row indexable cutter for 8 TPI. It sounds like you have design control so just make the crests and roots to clear.

Another option just use a UN form instead of NPSM. The thread height as cut is less because truncation is more. Just decide your major diameter to fit the pipe and pick a big 8 pitch thread, whatever you can find limits for. The difference in the major diameters can be applied to pitch diameters and minor dias to create your custom thread, and no sharp tools. They suck in SS.

 

[draganm]

i have finished these parts, and just wanted to say thank you to everyone one more time. In the end the male thread was pretty uneventful, molly D smoked like crazy and i huffed my fair share of it, but the thread came out really nice. No chatter, right on the mean dia.I wanted to try the bacon grease but ran out of time, smoke maybe less toxic? This is a big thread, your dialing in .094" on the compound at 30 degreee's to yield an .081 tall thread. I took the first 5 passes at .005" on the compound, then .003, then .002, and finally the last .01 or .015" i was taking .001" depth of cuts.

What gave me a little trouble was the Pipe ID bore. The pipe is not round, it's not only .015" ovalized but also "lumpy" for lack of a better word. I could not rely on the 3-point steady rest to do the ID. For me it was
1) set 3point rest as tight as possible without binding the bearings
2) face end of pipe flat, lightly chamfer ID at 30 degree's to match tubing live-center.
3)engage live-center
3)skim cut OD round
4)slide rest down onto machined OD
5) bore Id
6) re-engage live-center- cut threads.
Hassle but it worked well.

For the load bearing rings, i went ahead and turned them. Not nearly as smoky as the pipe, a little chatter, but no big deal ( I used a 1.0" boring bar, could have been bigger). I held this down to the minim. pitch dia., and maybe a little too tight, but they spun on effortlessly with no binding = good enough. Engineer gave the thumbs up

My big Colchester Copy, 27" x 60" with 12" chuck

final assembly

 

[michiganbuck]

QT: olly D smoked like crazy and i huffed my fair share of it,

So was the greatest fix the lubricant?
RE; (I'm using an NT3 Top-load like eKretz talks about. )
or changing the insert?

 

[john.k]

No doubt speed is the secret.....Ive got a machine that can single point thread at 3000 rpm,and its near impossible to get a bad thread,use the same cutter in a lathe at 100rpms ,torn and daggy thread,no matter what you slop on it.....The need for speed!

 

[draganm]

QT: olly D smoked like crazy and i huffed my fair share of it,

So was the greatest fix the lubricant?
RE; (I'm using an NT3 Top-load like eKretz talks about. )
or changing the insert?

from what i could observe, the Moly Dee oil made the biggest difference. Having that heavy oil with (presumably) Molybdenum additive is key. It really keeps that high pressure shear zone from welding material to cutter.
Second is speed, I trippled my spindle speed but unfortunately, still only half of recommended by machinist handbook (drawbacks of manual lathe). You need the correct surface-feet speed to create enough heat at the shear zone for good cutting.
I think tool is very important, but what i started out with was just a poorly designed tool, so hard to quantify. I loved the FT3 top-load, even though it's not the latest tech. That design is solid, very rigid, and the same edge did both ends of my pipe, about 60 inches of linear thread total. There was no edge breakdown after that much cutting either, with just the slightest hint of BUE. the male thread looked gorgeous, 32 finish or better.
the female thread was a little weird, i might not have done it the best way possible, but it worked. I wound up flipping the tool upside down and threading on the backside of the bore (spindle turning towards operator). This way, when i turned my compound in, the force of the cut was pushing the insert back into the holder.
To do it with tool facing up, operator side of bore, your dialing the compound out instead of in, and insert is pushing on retaining clamp.
Maybe this is not an issue, but i did what makes the most sense to me. Any rate it's done, hooray

 

[draganm]

i just looked, Molly Dee owned by Castrol now? and $69. for HALF a QUART! holy crap. This is nuts

yesterday i paid $227. for a 5 gallon bucket of water soluble machining coolant :O . Granted it's very good stuff, coolant in my CNC mill is 5+ years old, but dam!