[CitizenBrian]

I was wondering what everyone thinks is the best method for machining an O.D. thread. Single pointing is the only thing I currently use but we have a job coming up that may benefit from a different method like thread milling or thread whirling for example. The only print I could pull up was the part that had a 1/2-13 thread on it but I know there are smaller ones as well. These parts would be running in a L20 and an A32 and made from 1144 stress proof.

Thanks

[txcncman]

Thread whirling? That is a new one. Mind if I use it? I think you mean thread rolling or thread forming.

The best method depends on soooo many factors, one could not fully explain in a life time.

Size of thread

Length of thread

Type of thread

Specifications of thread

Final use of thread

Type of material

Machines available

Horsepower available

Tools available

Rigidity of work piece

Coolant/lubrication available

[CitizenBrian]

No I meant thread whirling (Genevieve Swiss Industries - Tooling & Accessories for Swiss-Type CNC Machines - pt#cit-btw100-u9.1) Now I have never used one of these before and I've only seen them used for bonescrews but I'm told they can be used for normal threads too. I know there are many factors when it comes to threading, I'm just looking to see what method others prefer in general.

[txcncman]

Ok. Looks like segmented die threading to me. They probably call it whirling to "brand" it and trademark it for their products only.

On a lathe, my preferred method of cutting OD threads is single point threading. One tool covers a large range of threads.

On a mill, my preferred method of cutting OD threads is "single point" thread milling. One tool covers a large range of threads.

My only consideration for varying from these methods would be extreme difficulties encountered using these methods or if production numbers were so high that the per part time savings would justify the additional tool cost and set up time to switch methods.

[SirDenisNayland]

Never heard of thread whirling? You've got to be kidding me :haha:

[txcncman]

No, I was not kidding. Found it after some digging:

Marubeni Citizen-Cincom, Inc.

"There’s not much new about whirling. It’s been used in Europe to machine helical parts for more than 50 years. It’s time-tested, and it’s proven to machine screws and thread forms at speeds often as much as four times faster than traditional thread milling or hobbing, and typically without the need for secondary finishing operations. But that’s in Europe.

What’s new is whirling’s recent and growing acceptance in the United States. It has become widely used in the manufacturing of “large” parts, such as steering gears, worm gears, acme threads, ballscrews and other threaded parts. To make these, however, has required installation of large, costly and dedicated whirling machines.

Now there’s an alternative. It’s a new whirling attachment that’s designed specifically for use on Citizen-Cincom Swiss turning centers. This new tool brings the advantages of whirling to the production of “small” parts, such as bone screws and threaded surgical implants. It also introduces this new application to a non-dedicated machine tool, while preserving the machine’s multi-axis turning, milling and drilling versatility."

Looks like Star also has a unit available.

I have never operated a Citizen-Cincom Swiss turning center. I have never worked for a company that had a dedicated whirling machine. The required tool looks to be very expensive and the initial set up quite time consuming. Definitely looks like something I will avoid unless I start getting machine screw orders of 10,000+ per year.

[statescrew]

Yep, it's thread whirling and it does a great job if you can afford the attachment. Think of it as turning and threading at the same time and smooth threads , no burrs at all. As an option over single point threading outside of that, we have used geometric dieheads. Much faster even at lower rpm's but, not as nice as single pointing. Just use it like your rigid tapping or floating. I find chasers to be sub par these days and it really effects how the dieheads work. Hope this helps?

[MikeMc]

We roll a lot of threads here, and it works great. Unfortunately a 1/2-13 thread is way to big to roll on an L20 IMO. Whirling might be the way to go if you are making a lot of the parts.

Well....I just looked at Genevieve, their whirling attachments for the L20 are 12mm and below, so it looks like 1/2" thread is out. They don't sell the attachment for the A20.

[micky316]

Is it possible to turn the blanks then get them sub contract thread rolled on a horizontal thread rolling machine ,normally quite a cheap 2nd op and always looks good if you cant roll on op 1

[gizmo_454]

Is it possible to turn the blanks then get them sub contract thread rolled on a horizontal thread rolling machine ,normally quite a cheap 2nd op and always looks good if you cant roll on op 1

This would be a great option, if and only if, there are no axial holes in the part. Rolling the threads of, say, a socket set screw will crush the socket, if they are rolled as a second operation.

Also, you would have to take into account part elongation when the treads are rolled since the rolling process displaces material. The part will grow in length.

Mike

[CitizenBrian]

Due to some of the parts being too large in diameter for our L20 I think I am going to run all the different parts in our A32. There is no whirling tool available for this machine yet so it looks like thread rolling is what I'll be looking into now. The parts do not have an axial hole so crushing will not be a problem. As for rolling as a second op we really try to avoid any 2nd op's cause with the additional handling of the parts comes the risk of scraping them.

[gizmo_454]

If the parts are all of a standard OD, why not just single point them? As I am typing this, Our Citizen E32 is chugging along making M16x1.5x59mm socket set screws. They are about 2-5/16" long. No second op threading. The idea behind the swiss is to keep the second ops to a minimum.

As to rolling the threads, you can try that. You mentioned 1/2-13 as one of the possible threads. I'll tell you that I thread rolled M12x1.25 threads in our 15HP Haas SL-10 lathe. The material was A-311 Stressproof. It did it, but it was quite a load on the spindle. 1.25 pitch threads are roughly equivalent to a 20 pitch, and M12 is smaller than 1/2". Let me know how it goes! I would be interested to see.

Mike

[TheKid09]

I thread whirl daily..
It is an AMAZING way to get a really good, and constant screw.
Only thing that will get you is the inserts..

I would recommend using the G32 command if you do try it...especially if you have to come back into your thread...using the C-Axis for this is REALLY hard and tricky..

[PixMan]

Before you go off on tooling up for thread whirling or thread rolling, tell us more about the task at hand. The requirements of the job are paramount in the world of sliding headstock machines, as in how many do you have to make, what is the cycle time goal, what machines are available, will the job repeat, and so on.

I find that many times when people go looking for a different way, they've overlooked examining just how inefficient the current process may be. For example, if there is one major, almost ubiquitous deficiency I find in single-point threading it's in selecting the right tooling (often just the right insert) and the number of passes.

I'd guess that perhaps 1 in 20 CNC Swiss-style machine programmers has ever looked up the recommended number of passes for any given thread pitch, selected the best insert for the job, optimized the cutting parameters, pre-turned the correct diameter, and more.

The 1144 stressproof materials is BUTTER to cut, especially in oil. With the right full-form cresting insert, a 1/2-13UNC thread should be done in as few as 5 or 6 passes in that material. With newer machines, the right insert (with today's grades and coatings), you should be able to reliably thread at speeds of over 2000rpm and in some machines, over twice that. Use the tools, they last longer!

Another option I don't see mentioned is Geometric die heads. Those can cut the thread in one pass and be the second-fastest way of making threads. I would think that only rolling in a flat die machine as a secondary operation could be faster.

How many of these threads need to be made, over what period of time? How many spindles are now making them? Has a multispindle machine been considered?

I've done some thread whirling, thread milling and thread rolling (that in both on-machine roll die heads and on flat die 2nd ops.) I find that Geometrics are the quickest. Single point threading (done right) is good for reasonable cycle times in the lower-quantity parts or in the no second op possible situation.

Give more info info about the thread requirements and we can collectively help find the most cost-effective solution.

[CitizenBrian]

I had the Fette rep come out to our shop the other day and he is going to set us up with a thread rolling tool to use for a few weeks for free, all we had to do up front was buy the thread rolls. We are starting with 300 pieces of each of the following threads then we will be doing thousands per month of each one.
3/8-16
1/2-13
5/8-11
M10x1.5
M12x1.75
M16x2.0

[PixMan]

If you're doing thread rolling on a Citizen, you may soon find the limits of spindle torque on those machines. While it should be able to roll the 3/8-16 and perhaps the 1/2-13 and M10, the coarser threads may need more than what the machine has available.

[SirDenisNayland]

Tip: if you must run a specific thread on a specific machine but it doesn't have the torque to push out the whole thread, peck threading is an option. I've done it with taps, don't see why it couldn't work for other phased threading applications.

[gizmo_454]

If you are going to peck thread, of which peck tapping is usually used for clearing chips out of deep holes and not power related issues, you are back to burning more time than it is worth. You might as well be single point threading. As Mr. Scott once said on Star Trek, "The right tool, for the right job!" In this case, if the threads needed to be rolled, and the machine didn't have the torque to do it, then a bigger machine or different approach would need to be taken. Since he has been open to discussion on different approaches to the thread, on the parts that can be rolled, by all means, do so. On the ones the machine cannot do it, by all means, single point it, thread it with a Geometric die, or many others.

Peck rolling would NOT be my choice. Rolling inherently cold works the material, effectively work hardening many materials. Once you try to go back over it, it may destroy the tool.

Mike

[SwissType1]

A full profile true Swiss-style threading insert might do the trick here and certainly is a lot less expensive than a dedicated head or special attachment. Full profile inserts should generate extremely clean threads in that material.

UTILIS makes a 1/2-13 full profile threader in their 3000 series product line.

-Scott@Genswiss

[SirDenisNayland]

@gizmo

You're right about the work hardening aspect, probably would not be the best for all types of material.

I just thought id throw it out there for anyone who hasn't used or thought of it before. Like I said if you're constrained to a specific set of conditions you can't change, it may just be a life saver.

I've used it tapping a rather deep 5/16-18 thread in the sub on an L20 where it kept stalling, tap was fine, chips were evacuating but the machine was at its limits for sure. It was 304 iirc, and an id single point would not have lasted at all. That small a bar as deep as it had to go would have taken a retarded amount of passes, not to mention 304 work hardens if you don't take a deep enough cut. Peck tapping was definitely the best option for me at the time :bigthumb: