2-56 UNC 3

You didn't say what type of tap are you using? I'm hoping it's a fast sprial 4 flute. I'd also change to a # 48 drill, the added diameter will assist in the chip removal, Titanium will be a bit stringy and bind up that small tap. (the extra .006" diameter is with the tolerance of the thread allowed, meaning the no go still will not go).

let me know how that works out for you

Hello,

The number 50 drill per a tap drill chart such as:

http://canstampconsulting.com/ezine/tdsdrillchartmgc.pdf

will give you a thread percentage likely 73-78% of the tap diameter, which is recommended for most tool steels and also works well on mild steels for the majority of holding strengths of tapped holes, of course the holding strength of the thread is the bottom line as per design.

Tapping small holes in Titanium likely requires a larger diameter tap drill (this diameter should be established as per calculation, taking into consideration the depth of the hole and the material characteristics, and forms a base for the holding strength of the thread)

The depth of the hole in relation to the diameter does seem exaggerated - do you know what the fastener to be used in these threads is made of? The reason I ask is that at some point of depth of thread engagement the fastener would fail before the thread you tapped fails, thus affecting the true required minimum depth of the hole that needs to be tapped. If the drawing does not specify a thread pull out value, this may not be as critical, and you may carefully inquire to be allowed to reduce the thread depth, any reduction in depth will help.

Most important factors for any small hole tapping operation and no different here:

Spiral fluted tap if possible to get the chips out.

Correct tapping fluid for your application.

The correct cutting rake angle of the tap for Titanium, perhaps relieved on the back side - carefull if grinding yourself -temper it properly, grinding induces stress!

Sufficient tapping fluid on the cutting edges.

A high quality tap from one of the top manufacturers is important.

The correct coating on the Tap in conjunction with the cutting fluid.

For titanium you likely also want a coated Tap, although the coating may be similar to the material you are tapping into - titanium carbo nitrate coating - on this just ask your TAP supplier, or a new supplier that is eager to solve the problem with you and assist you. Tap manufacturers and suppliers usually have connections to special labs which likely already hold the best answer or can test your part.

What you should find out first is what minimal thread % will be acceptable by the customer, which can also be proven per the thread pull out requirement which may actually give you advantage if it is not stated on the customer manufacturing drawing. Of course the larger the hole the easier it is to tap.

If you have to tap a very large number of holes assure to use a proper fixture to set up the parts and a rigid milling machine, perhaps with a special tapping head which auto reverses, getting rid of the need for speed and feed - this may be impractical due to overall cost and the size of the thread - it is just a phone call to find out from the tap head manufacturer if they have knowledge in this direction, perhaps also to demo a head for you on your parts.

Another question is: is a blind hole really necessary here? I have seen cases where junior designers have added blind holes to parts without the regard for manufacturing or maintenance.

Personally, I rarely design anything with a blind hole as it is a recipe for high manufacturing costs as well as creating issues for maintenance and repair on that item as well should a broken bolt be encountered. Of course in some cases this can`t be avoided.

Best of luck, be sure to post how you solved your particular problem!

I hope this helps!

Mirco

Try using a roll form tap. You get no chips and can tap nearly to the bottom of the hole. TIN coating on the tap works well for wear resistance. Use Moly-Dee cutting fluid made by Castrol. Your standard tap drill size for 2-56 is 5/64, but you may have to adjust that a bit one way of the other. I assume by the UNC 3 designation you mean that it is a 3B tolerance thread. If so you may want to run your tap drill size down to 1.95mm. If you are breaking taps you may have to go up to #47 or 2mm.

Your tapping speeds are not quite as relevant as the above issues. For a tap as small as 2-56 you could run it very fast, but most tapping heads are not designed to run above 1000rpm, so you are not likely to go too fast. If you are tapping in CNC the issue will be with your machine and whether or not it can stop the spindle and reverse it without running the tap too deep. Also to consider is your tool holder and if it is running concentric. If not with such a small tap you will get a lot of breakage.

Most of the tap companies have applications people who will help you if you call them. I once had a guy from Balax come out to my shop and consult on a tapping job and he was great. I hope this helps, and good luck.

Gary

Hi Gary,

1000 rpm? that seems fast, but I am eager to learn.

I came up with 690 rpm max, and realistically I feel that this is way way to fast for a blind hole, in fact I would try to run the tap at no more than half that speed for the first trial run.

I tend to think that using a roll form tap is only feasible if this is a form tap with a relieve cut to remove minor amounts of excessive titanium which would otherwise cause that tap to seize. Have you tapped small holes in titanium with a # 2 forming tap? I have not, but based on other tough materials, I am fairly certain that the titanium will cause it to seize in the hole.

As per the machineries handbook the MINOR diameter limits FOR THE FINISHED thread are .0.0667 to .0737" how will you attain that with a 5/64 drilled hole (.07813"), in a formed thread I can understand that this diameter can get smaller by material moving to toward the center during forming, but you were talking about cutting in that sentence, right?

You would likely have a better chance by drilling the hole .0595", then reaming it with a custom reamer to near the max size .0700, reaming at no more than 500 rpm with plenty of coolant and a carbide reamer at best.

Gary I agree with you, to get a tap manufacturer and expert on it. Try to get help from OSG or Greenfield tap manufacturer they have extensive labs, and likely have been aproached with a similar problem before.

Another thought - is there a way to anneal work hardened Titanium?

I am eager to hear what finally worked here, as I am all tapped out here!

Hi Gary,

I can tell you are very knowlegeable on the subject. I have had my share of roll form and conventional tap stories - in some of those stories the end fell off! At the end of the day the parts were always done! I am eager to learn more about working with titanium.

Now we just have to wait and see how the "guest" made out with his parts, and hopefully learn something. I think the info you provided deserves a "good answer" overall and I have voted, I hope some others will follow.

All the best, also to the "guest".

Mirco.

Your problem is magnified by the need to use a 2-56 thread. The small size of that tap is a problem with any metal tapping job. Taps of sufficient strength are just not readily available in that small size. Do you really need a 2-56 thread? It would simplify things if a larger thread could be used, necessitating a redesign of the part. Could you use an insert, say .125" dia of a softer material and tap it for the 2-56? An insert made by powder metallurgy could be used.

Thanks for the education, something I didn't realize.