Why is "thread milling" not a common practice in lathe work?

[CalG]

Although the process would require live tooling, It would seem to offer many options regarding materials and thread form.

Whirling would be a most similar process, which is used for feed screws of many types.

Maybe the process is used, and I just haven't run in the right circles.

 

[Danny VanVoorn]

Cal,
I have thought about that myself for an engine lathe. Building a suitable driven spindle and the right set up and hardened steel could be threaded. That is nearly impossible with a single point tool but not with a carbide thread mill; seems like a worth while endeavor?
San

 

[iMillJoe]

It's my experience that while live tooled lathes can mill, the c-axis one are not very good for milling straight lines, or circles, or anything to close form. When the machine transitions from feeding in with the x-axis, to feeding out, (or vise versa) while rotating in C, it seems to always leave a bit of an error. I could see thread milling being handy for threads that were on center but tricky enough to warrant milling. With a c-axis lathe, trying to thread mill a bolt hole pattern with an 8" diameter, might be tough, if even possible. I don't know if y-axis lathes have this same problem, I imagine not, but most have very limited strokes in Y.

I have a part I'd like to start making that would involve thread milling. I've yet to get the chance, but if I could prove I can make it, I might be able to talk them into getting me a fancier machine to make them with.

 

[yardbird]

I wish I a nickel for very time I wished I could circle jerk a 1/8-27 NPT for perk holes in hardened tool steels.

I very much do so at times would like to have that option, no doubt about it.

In softer stuff its just as easy to single point it plus I doubt I'd be able to get the depth on larger threads that's required?

Brent

 

[CalG]

Nothing to stop one from making multiple passes.... except machine capabilities.

 

[Comatose]

I've done it on a Y axis Okuma. Worked fine.

I'm skeptical that you can really get more options regarding thread form and material. I did it because I needed threads right up to a shoulder. No space to undercut, no space to fade the thread and couldn't accept the torn last thread you get with an abrupt stop single pointing. Multi-tooth thread mill worked a treat.

But, it uses up one of your live tools, a thread mill costs an awful lot more than a threading insert, likely slower.

I don't think the issue is so much that it's unheard of as it is that only comes into play once in a while, and if it does, it's either a thing you can do (and it's really no big deal at all after the first time) or it is a thing you can't do (no live, no helical interpolation) in which case why talk about it.

 

[CalG]

Comotose

If you note, this idea was not posted in the CNC topic forum. The idea of "thread whirling" applies to any lathe that will cut threads. No interpolation required! ;-)
Some materials MAY be better suited to small chips than single pointing.

Certainly large and coarse thread forms on smallish machines could take advantage.

 

[JRIowa]

Maybe the process is used, and I just haven't run in the right circles.

Go to a mold shop and watch them make inserts for OD threads and "threaders" for ID threads. Used to make the parts on a 15" Colchester. Most would laugh at the set-up we had then, but it worked. Most everything was shop made except for the taper attachment on the lathe. I loved polishing those threads even more than cutting them. IIRC we had a pulley set-up to get the lathe spindle down to 4 or 5 RPM.

Way back in time, I did the molds for these : M-2 Yard Hydrants | Merrill Manufacturing
Just the "head" had 4 ID threaders and 1 OD insert.
JR

 

[rustyhunter]

Hey guys, hope all is well! I came across this thread and joined the forum to chat about it. Thread milling is something I always try and do on the lathes when I get the chance. We do not have a Y axis on our lathes so I always found it tricky finding out information on how to thread mill a PCD on a lathe. Anyway after thinking about it for a bit I made a macro to do just that, I have used it for months on the shop floor and it works every time without fail. From 1/2” holes on a 6” PCD right up to 3” holes on a 20” PCD. It has saved me from so many bottle necks on the borers. Anyway I thought you guys might be interested to know that it is possible and reliable to do it in a lathe. I’ll post a link to a video I posted of it working, feel free to ask if curious about it. Russ
Link Russell Hunter on LinkedIn: "No Y axis? No problem! An example of a Macro program that I made to help take some of the strain off of the horizontal borers. Drilling and hobbing a PCD using the Z X and C axis on one of our lathes. When capacity on the borers is an issue you have to work around it. This way we get to add to the skill set of the guys in the shop and we also keep our customers happy. The video isn't the most exciting thing in the world but the end result is, for a CNC geek like me anyway #Macro #CNC"

 

[FredC]

Old thread that I missed the first time around. So I will add to it now.
I have a 97 Hardinge GT and called them to ask if the spindle would run slow enough to mill small threads. The engineer did not think so since it did not have C axis. He expected the spindle would not run smooth but would buck.
I tried it anyway as I needed to thread behind a shoulder to get the threads and a bore on the front of the part 100% concentric. It worked like a champ, also worked on a .080 long 3-56 nut, and a longer small diameter part that would have been difficult to single point. All are repeat jobs. It is slower than single pointing, but for difficult parts thread milling sometimes is the answer. If anyone is interested this GT will run smooth 15 to 20 RPMs. Have not tried to find a low limit, so I do not know if 15 is it or if it will go slower.

 

[rustyhunter]

Old thread that I missed the first time around. So I will add to it now.
I have a 97 Hardinge GT and called them to ask if the spindle would run slow enough to mill small threads. The engineer did not think so since it did not have C axis. He expected the spindle would not run smooth but would buck.
I tried it anyway as I needed to thread behind a shoulder to get the threads and a bore on the front of the part 100% concentric. It worked like a champ, also worked on a .080 long 3-56 nut, and a longer small diameter part that would have been difficult to single point. All are repeat jobs. It is slower than single pointing, but for difficult parts thread milling sometimes is the answer. If anyone is interested this GT will run smooth 15 to 20 RPMs. Have not tried to find a low limit, so I do not know if 15 is it or if it will go slower.

Good work bud, you never know until you try. Always love problem solving with cnc work, even trial and error until you get what you need

 

[EPAIII]

Interesting thread. I would love to see some photos.

Also I am curious about all these lathe axes. C axis, Y axis, etc. Just what are they?

 

[litlerob1]

Hey guys, hope all is well! I came across this thread and joined the forum to chat about it. Thread milling is something I always try and do on the lathes when I get the chance. We do not have a Y axis on our lathes so I always found it tricky finding out information on how to thread mill a PCD on a lathe. Anyway after thinking about it for a bit I made a macro to do just that, I have used it for months on the shop floor and it works every time without fail. From 1/2” holes on a 6” PCD right up to 3” holes on a 20” PCD. It has saved me from so many bottle necks on the borers. Anyway I thought you guys might be interested to know that it is possible and reliable to do it in a lathe. I’ll post a link to a video I posted of it working, feel free to ask if curious about it. Russ

Not to burst the bubble, because it's cool! But Threadmilling without Y isn't new, and this Thread was about Manual Lathes. Any decent CAM program will substitute C for Y in Turning. If you want to try something interesting, do flats on the OD, with a Milling tool perpendicular to the main Spindle without Y!!

R

 

[FredC]

Did not know that milling flats with out Y would be that interesting.

Attached photo shows the thread milling mentioned in the earlier post.
On the parts on the left the nut was made in one operation from 3/16 round bar. The shafts were done in 3 separate operations with the bore the stainless tube is mounted in being the 2nd, the slot 3rd.
The parts on the right, the stud on top shows finished 1st op and the finish assembled part minus the O-rings. The stud on the right was also made from round bar. As mentioned earlier no Y, or C axis, the machine does have spindle orient.
Each part was thread milled for a reason, conventional threading is usually faster. I will say that milling is more accurate. We could make the threaded stud drag on the go gauge for the entire run.

For size relationships the nuts on the left are 4mm hex with 3-56 /2.5 X .45mm threads, the gauges are about 80% interchangeable.

 

[litlerob1]

Did not know that milling flats with out Y would be that interesting.

That's just because you haven't tried it. Here, try this part without Y on a Lathe. The top one with wrench flats.

 

[FredC]

Yeah, those flats go the wrong direction for me. I would need a Y axis to do them.

 

[litlerob1]

Yeah, those flats go the wrong direction for me. I would need a Y axis to do them.

Actually you wouldn't, that's why it would be interesting, right?

 

[FredC]

Actually you wouldn't, that's why it would be interesting, right?

If you have a solution, I would love to see it. I could use it on tomorrow my next job.

 

[FredC]

Robert your mail box is full. I just saved a bunch of my messages in text files then cleared it out.

 

[Lumberjack]

FredC,
It´s not classified info, just google polygon turning.
Polygon Milling - YouTube