Thread Rolling in Titanium

I need to roll some threads in a blind hole in 6AL-4V titanium. They are about 5/8" holes, about 5/8 deep. Anyone have some guidance on how to do this?
Thanks,

--
J Kimmel
snipped-for-privacy@whereIwork.com
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
Thread rolling is normally used in the making of external threads, as on a shaft, for example. It is a lower quality thread than a cut thread. Inexpensive threaded rod that can be purchased in a hardware store is the best example I can think of to demonstrate rolled thread quality. It is generally used when the cost of the item needs to be as competitive as possible. You can cut the threads that you need very easily, by drilling a 17/32" hole, 5/8" deep for a 5/8-11 thread, which is standard, or by drilling a 9/16" hole for a 5/8-18 thread which is a fine thread, then using a starting tap, followed by a plug tap, for the last few threads at the bottom of the blind hole. If you require a lot of holes to tap, you will need "coated taps", and a good quality lubricant, as Titanium, is about as tough a metal to machine as you will find. I hope this helps you.
G. De Angelis Valhalla Grafix www.deangelistool.com guynoir wrote:

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
I would take slight issue with you on being an inferior quality. Rolled threads are used on high tensile bolts due to the grain flow it produces, therefore yielding far greater strength. Aero engine bolts are rolled and ground. The inferior quality may certainly be attributed to the final form, therefore the follow on grind operation.
---------------------------------------------- Posted with NewsLeecher v1.0 Final * Binary Usenet Leeching Made Easy * http://www.newsleecher.com/?usenet ----------------------------------------------
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
On 12 Jan 2007 14:29:53 -0800, "G. De Angelis"

Boy, someone gave you some misinformation.
Thread Rolling is Superior in many respects:
Depending upon material but here are some highlights and advantages for thread rolling.
Thread rolling is widely accepted as the fastest and preferred method of economically producing uniform smooth, precise threads of superior physical qualities.
In penetrating the surface of the blank, the rolls displace material to form the thread roots, and force the displaced material radically outward to form the thread crests.
Strength
Cold working of metal during thread rolling improves thread form physical characteristics and mechanical properties. When thread is rolled, the structure is deformed and the surface is hardened. Increased surface hardness results in thread form properties that are superior to those of the original material.
Grain structure is maintained with rolled threads, in continuous unbroken lines following contours, increasing tensile and shear strength.
Improved Finish
The smooth flanks of rolled threads provide better surface contact with mating threads. The burnished roots and flanks are free from chatter, tearing or cutter marks that can serve as a focal point or stress and starting point for fatigue failures.
Accuracy
Rolled threads maintain consistently closer tolerances and uniformity than cut thread. Thread rolling is unique in its ability to maintain accuracy of the original set up during long runs of high-speed production. Dies do not change appreciably during the life of the rolls. They do not wear like other types of threading tools.

What you see at a hardware store is commercial grade probably a 1A tolerance or even a looser application. As well as the rods in the hardware store are handled none too carefully.
FYI, a lot of aerospace fittings and fasteners require rolled threads because of increased thread sheer strength and quality.
Tom
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
I have a tap sitting on my desk that rolls internal threads.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
TOP wrote:

How about posting a photo of that? My main question(s) are: is it adjustable and is it common practice to make more than one pass to roll the thead?
--
John Kimmel
gNuOy snipped-for-privacy@sNpOiSrPeAtMech.com
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

<http://www.emuge.com/taps/gfu_druck.html
It's a one pass operation.
I don't have the pitch nor my technical data handy, but I'm guessing without a geared head spindle you'll need an honest 15-20 horsepower depending on the pitch. Or about 30-40 haaspower.
--

Dan

CNC Videos - <http://tinyurl.com/yzdt6d
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
I wouldn't want to bet I could do it.
Titanium (alloys do differ) generally work hardens and that can make for some humongous forces and at some point you can exceed the ultimate strength and just fracture the metal.
Bo
D Murphy wrote:

Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
D Murphy wrote:

I found a picture of a roll forming tap. It was not what I thought, I expected "rollers". It looks to me like you just drive a screw into the hole and create threads that way. Now I understand why it takes so much torque and why you need "venting".
Cut threads are not an option. It is a very high stress, very high fatigue forged aircraft part: a helicopter tail rotor.
Thanks for all the excellent information, I may be asking for quotes.
--
J Kimmel
snipped-for-privacy@whereIwork.com
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

=================see http://news.thomasnet.com/fullstory/476363/1292 http://findarticles.com/p/articles/mi_m0KJI/is_8_113/ai_81138590 http://www.emuge.com/taps/gfu_druck.html http://www.emuge.com/technical/tapfinder/drucksticn.html http://www.emuge.com/technical/tapfinder/druckpmticn.html and many more.
Because of the high force/friction involved in internal thread forming in titanium, your choice of tap lubricant may be critical. Some of the best friction reducers such as MolyDisulfide may also contaminate the metal.
Has anyone tried a lube containing teflon?
Good luck and let the group know how you make out.
Unka' George [George McDuffee] ............................... On Theory: Delight at having understood a very abstract and obscure system leads most people to believe in the truth of what it demonstrates.
G. C. Lichtenberg (1742-99), German physicist, philosopher. Aphorisms "Notebook J," aph. 77 (written 1765-99; tr. by R. J. Hollingdale, 1990).
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
On Fri, 12 Jan 2007 17:37:44 -0600, F. George McDuffee

Good point. Probably have a bit of trouble if you try to use toilet water :-). I use CutMax 570 cutting OIL, which has a rather high sulfur and chlorine content. The largest roll tap I've ever had the chance to run in TI, was a 3/8-16. It was a while back, but IIRC, I ran the entire 350 pc. order with one tap.
Matt
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Rolling ID threads is not a problem. Do it all the time. You simply need a roll tap, or also referred to as a Thread Forming, Cold Forming, or Roll Forming Tap. You can start by using it just like you would a cut tap, although you will most likely find that you can run it at a faster rpm.
You're going to need some HP behind that tap. Don't know what kind of machine you're using, but I run 1/2-13 roll threads on my 5C Gang Lathe rather often, and it works quite well. It groaned a bit the last time I used a 5/8" CUT tap, and, although I've never tried it, I'm quite certain that it wouldn't pull the 5/8" roll tap. But then, it's pretty wimpy. Hopefully you have a machine with plenty of power.
Find some taps with oil grooves. You're going to have enough fun without having to deal with the hydraulic resistance of the oil compressing in the bottom of the hole. The Greenfield taps have 4 oil grooves, and really do work well. Some of the local (Escondido/San Diego) tooling suppliers stock them, but you can also get them from McMaster Carr or MSC. OSG taps are another good choice, but I don't know if their larger diameters have oil grooves or not. The 1/4-20's I have here do not.
Matt
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Guy,
Does the print REQUIER rolled thread? If not your going to need some horsepower, a very good setup and very good lubricant.
When I use to roll external threads in titanium years ago we needed to use an induction heater and roll them hot because the machines HP could not do it cold depending upon the thread size and length.
In my opinion it is almost always easier, better and faster to cut titanium than roll it.
Tom
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
51g2000cwl.googlegroups.com:

If you have a choice, thread mill. Otherwise cut tap. Only use a roll form tap if the drawing requires it. Assuming you need to roll form the threads, you need to consult a tap drill chart for roll form threads. The tap drill size will be different than a cut tap. It should be right around the pitch diameter. For best results use as low of a thread engagement percentage as is allowed. IOW, use the largest tap drill size that is permissable.
Also if the drawing calls for a tight tight tolerence on the thread, then you should ream the hole before tapping. Probably not a bad idea in any case.
Run the roll form tap at around 20 SFM or so for 6Al-4V. Use a cutting oil if possible. If you have to use water soluble, make sure it has an EP additive in it. If you are doing this on a VMC consider putting a cup of oil or tapping fluid on the table somewhere out of the way, then dip the tap into oil before tapping. Or seeing as they are blind holes, you can program an optional stop before tapping and fill the holes with oil.
I hope you have a machine that has some serious low end torque, especially if it's a coarse pitch thread. Otherwise don't even bother, you'll stall the spindle.
--

Dan

CNC Videos - <http://tinyurl.com/yzdt6d
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Good advice.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Related Threads

    Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.