Tapping Ti.. What is the secret?

J S Machine

Well-Known Member
I love Ti as a material for my knives but the stuff is very hard to work with. I have trouble drilling, sawing, and tapping it. I don't seem t have any problem cutting it in a mill with end mills though.

What I've come here to settle today is how I should be tapping it. I really need some help with this. As a tool maker, I have tapped literally thousands of holes in all types of material. In other words, I am not an inexperienced person..

However, Ti seems to break my taps with ridiculous frequency. I usually cannot get but two or three very small holes before the tap breaks. Something about Ti that I can't really explain..it's like it shrinks around the tap or something. Even though I'm using a brand new tap, and a few different kinds of cutting oil, I still get unreal friction. It feels like I'm tapping a hole that is drilled under the tap drill size called for, but in reality I drill it bigger just to avoid this symptom. It still feels tight.

I always use good name brand taps. I try to stay away from the cheap Chinese junk.

A look at the tap chart says a 2-56 tap needs a #51 drill, which measures .067". I will step up to something like a #50 or even a #49, and I still get a really tight binding.

I posted this on Facebook last night and David Curtiss said he uses forming taps, not cutting taps. Is this the secret?

I need info ASAP. As usual, I'm stuck because I am right in the middle of making St. Jude knives for auction, and they have to be done by 8/1. I broke the last $35 2-56 tap I had last night on the second hole of .048" thick liner material. This is being done in a mill or drill press with dialed in tables..so the tap is straight. It is also being done by hand..not under machine power.

I need recommendations so I can get something ordered right away. Hopefully I'll get it within the week.

Thanks
 

EdCaffreyMS

"The Montana Bladesmith"
My "secret" is three fold......first and most important for me is the tapping head.....I have one from Enco that is mounted to a dedicated Ryobi 10" drill press. Next is the size hole you use/drill. I've come to take the information the drill/tap charts give, and go 2-3 sizes larger. In some cases I've even gone as large as 5/64" on thicker Ti. (for 2-56 threads) Third is the type of tap (as you mentioned)......for thread forming taps I use a #48 or 5/64" bit. If you use cutting taps, use a spiral point tap.

Something else that might help is....if you're using thick Ti (more then .100"), counterbore/countersink the "backside" of whatever hole you intend to thread.....and leave yourself only .050" +/- to tap. Even with a 49 or 5/64" hole, you will twist the head off a 2-56 screw before the threads will give.

If you don't have one, a tapping head is the way to go.....by hand, I used to break at least two taps for every folder.....now I wear taps out instead of breaking them. With the tapping head clutch properly set, you will get literally hundreds of threaded holes from a single tap.
 

J.Higgins

Well-Known Member
I always use cutting taps, and tap-hole sizes from the chart, and rarely break a tap. I always use a decent tapping fluid, a tapping jig, and a plug tap. For thicker Ti, I use a taper tap, which gives a more-gradual bite, and does a great smooth job. Avoid using a tap wrench... that probably goes without saying.

Beware that Ti will work-harden. I'm probably stating the obvious, but there is no real reason for any knifemaker to use anything other than annealed 6AL4V. When I started making folders years ago, I was picking up drops from ebay that Boeing employees were taking home and selling to make extra cash. I scored a lot of great pieces, and made a lot of knives from them, but there were many different grades of Ti in those goodie bags. Never again. I only buy from reputable dealers who can guarantee I'm getting what I am asking for.

I hope some of this helps. Threading has kind of been my passion since I was a kid. :happy:
 

Smallshop

KNIFE MAKER
That Moly-Dee is good stuff but messy and stinky (all that moly) shake it often. The molybdenum settles in the bottom. Do not hand tap with out a jig or starting it in a drill press or mill. Keep that tap wet!

Get out your machinerys handbook and go to the threading section. On any thread there is a tolerance to the "Minor Diameter" they will list the max and min the minor dia should go. Take it right to the high. The thread in Ti will be plenty strong with the minor at the high. could even probably go a couple thou over but I never have as all the Ti I have machined was for aerospace stuff and they check everything.

A two flute tap has the most chip relief but is the weakest. A four flute tap has much less chip clearance and is stronger. Three flute is in the middle strength-wise. Some taps neck down after the threaded portion so you can tap a bit deeper. Don't use those. A four flute spiral point with a straight diameter the whole length of the tap is a nice stout setup. The knife stuff is all relatively shallow so chip relief is less and issue than strength. Remember to "break the chip". clockwise a bit and then back off to break the chip that has started to form on the leading edge of the tap. If you let that chip get to long it can curl and wedge, breaking the tap or some teeth. Experiment with this. Try a half turn tapping then back off until you feel it break the chip (maybe a 1/4 turn) then forward again. If you are hand tapping with a jig use a good tap handle that stays locked and doesn't wobble on the square portion of the tap. Starrett makes a beautiful little tap handle for these types of jobs. Ed is correct that a tapping head is the cats meow and you can peck with those also. The reason I'm giving all the manual info is my small Tapmatic head cost just under $400 13yrs ago. But I wouldn't be without one if I was tapping a lot of threads.

On real small fine threads in Ti or soft stainless (321 etc) I have found that not guzzling coffee or caffeine drinks helps me not bust taps. Learned this the hard way many moons ago. I am dead serious on this one.....

Finally and most importantly.....DO NOT BUY IMPORT TAPS. yep that was a shout. It is a total false economy to buy cheap taps. Use something like Sossner, OSG, Greenfield, etc. There are a lot of good usa tap makers. You look at an import and , say, an OSG under a scope you'll see what I mean.

Hope this helps,
Ted
 
Last edited:

J S Machine

Well-Known Member
I did a bunch of reading yesterday, and I think I've learned a lot about the problem and the solutions.

first off, Ti has a low modulus of elasticity, so it has a “springiness". Because of this, it tends to “close in” on the tap. This effect causes galling and tearing of the threads. It also increases torque on the tap and is most likely the cause of all the breaks I've experienced.

A few solutions I have found make pretty good sense. Apparently, modern cutting taps have a pretty average rake in regards to the cutting edge, so that they will last. From past experience I know that positive rake cutting edges work best on softer materials, and I consider Ti to be fairly soft..softer than steel anyway.

The problem with positive rake geometry is that it breaks down quickly. a cutting edge with a more average or negative rake will be stronger and hold up over the long term.

In a nutshell, a slightly positive rake cutting edge will most likely do better on Ti, but then you have to deal with the dragging of the threads behind the cutting edge. The only way to alleviate this is by relieving the backside, so they don't drag..

So now that you have done that, the next issue is lubrication. I have used all sorts of tapping fluids and oils (never coolant), but some I have not used and saw mentioned repeatedly was this Castrol Moly Dee stuff. I even called Balax and talked to them, and their engineer recommended this stuff as well.

So if you wanted to use cutting taps, maybe the relief of the threads behind then cutting edge and good lubricant is the answer.

The other option is the thread forming taps. I have used these before, and we also have some that run in the automatic tap heads in dies at work, but I never considered them for this application until yesterday.

I knew that formed threads were stronger than cut threads, but had no idea they would be better for Ti. The reason formed threads are stronger is because the base material is simply rearranged, vs. being fractured and cut - removing material. The weakened material can develop stress cracks sometimes. If you can deal with he puckering of the material around the hole, you are good to go. The surface can always be brought back down flat around the hole.

Another plus to form taps is the increased material in the cross section. Cutting taps have significantly more material removed to create the flutes needed for chip evacuation, so there is less material there for strength. Form taps are missing very little, so they should be much stronger. They do work harder and take more stress because of forming the thread, but they should work fine with the proper size hole and good lubrication.

Something I also learned about yesterday was the use of tapping paste, for high friction situations. makes sense..kind of like bearing grease. They say it will stick around longer and provide better protection vs. an oil or fluid.

The Balax engineer recommended the form thread taps as well, so I'm going to give them a try. I also got some of the Moly Dee lubricant. I'll report back after.use and let y'all know how it worked out.

Ed- that's good advice about counter boring the backside of holes in thicker material. Thanks.
 

Frank Niro

KNIFE MAKER
Well I will add my day to day go ahead for tapping titanium. You can buy a tap holder that you place into your drill press and turn by hand . I used one of these for over ten years. The only time the taps broke were if after 250 or so holes the tap wasn't turning all that well but I forced it, or if I dropped this simple fixture on the floor. I now have an automatic self reversing unit I bought for about $250 new. I broke one tap when setting it up and just changed out the one I started with. For 0 X 80 I use a No. 55 for the tapping size and a No. 50 for 2 X 56 screws. The screws can be turned down over tight and they still won't strip out the threads in the titanium. I only make only liner locking folders with 12 to 18 holes for each. Frank
 
Last edited:

Smallshop

KNIFE MAKER
The moly dee works because the moly particles cut friction. If you use a roll tap or thread forming tap (same thing) you will get a stronger thread. you will also get deformation at the start and exit. Small but visible and will probably require some sanding or countersinking. When we say that thread forming is stronger that by no means implies that cut threads are weak. You would have to seriously over tighten a cut thread to strip the threads.

I used to mix lanolin and Moly Dee for thread forming as is stays on the tap better without running through. Heat the lanolin up in the microwave add some moly dee and stir.
 

J S Machine

Well-Known Member
I have not used the form taps yet, but I did get a chance to use the Molly Dee and a 4-40 tap. It was a cutting tap, so I relieved the back of the cutting edges (minimizing the amount of thread that is dragging through), and wow what a difference. The Moly Dee stuff really does work like they say. I've used all sorts of tapping / cutting oils, and this stuff is probably the best.

I'll report back after the form taps are used.
 

Smallshop

KNIFE MAKER
tap relief.jpg

There is no "dragging through" of the profile of a cutting tap. Otherwise it would be a forming tap (though they have a different sort of relief also, twist the forming tap between your fingers and you'll see they aren't round. The high spots do the forming). On the cutting tap the relief is already ground into the tap.(see pic on the left for standard cutting tap) What you did was merely weaken the tap and still get good results. That would lead me to believe that the main issue you were having is most likely not you, or the tap, but the cutting fluid. Perhaps try one of the taps you were having trouble with unaltered and see how it performs. A good rule of thumb I learned long ago was to only change one variable at a time. Then you know what actually made the improvement.

If grinding the tap did help over the unaltered tap then it is most likely a chip clearance issue in the flutes. I would try 3 flute or 2 flute taps then before altering as it will simply be more consistent than hand ground.
 
Last edited:
Top