[J S Machine]

I've been trying to figure out tapping titanium for some time and I have had a lot of trouble with it. Initially I was using very good YMW Japan made cutting taps and I kept breaking them. I did a lot of research and found that using form taps was the better idea and also using Castrol Moly-Dee CF cutting fluid.

I'm at a point now where I could really use the benefit of tapping in the machine but I'm not sure which way I should go. I know Tormach sells the tension compression heads but I've also had people recommend the Tapmatic heads as well. I do a lot of very small holes like 2-56 or 4-40 and they are blind holes.

Any advice would be appreciated. Breaking Taps is getting expensive. It is a weak point in my process that I have got to get nailed down.

[SCzEngrgGroup]

If you're breaking taps, then you're probably drilling the holes too small. Using T/C, Tapmatic, etc. is neither here nor there - the tapping process is the same regardless of how you do it. A tapping head will not prevent you from breaking taps. And tapping blind holes with a tapping head can be tricky, as you cannot tap to the bottom of the hole - you must leave room for the tap (and/or spindle) to come to a stop before reversing back out.

What size threads are you tapping, and what size are you drilling the holes? With difficult materials like Ti, you need to reduce the thread % to 50%, perhaps less.

Regards,
Ray L.

[J S Machine]

I'm mainly doing 2-56. Since I'm doing form taps, I'm doing the drill a formed thread calls for. It is a 5/64 (.078" or so)

[SCzEngrgGroup]

(Luckily) I have not had to deal with Ti, but, as I said, if you're breaking taps, you're doing something wrong, and most likely the hole is simply too small. I would go a bit larger on the hole, and see how that works. When you get to where you get a good, consistent result, then measure the threads, and make sure the fit meets your requirements. Also, with Ti, the tap coating, and proper lubrication are critical, to prevent heat build-up and galling, which can "grab" the tap. I would start by buying taps made specifically for tapping Ti, with good technical data straight from the manufacturer, and follow their recommendations to the letter. If you still have trouble, call the manufacturer, and get some technical support. You'll likely even get some free taps from them. If you're breaking taps doing it by hand, machine tapping will do nothing more than increase your efficiency - i.e. - it will break the taps MUCH faster...

Regards,
Ray L.

[SCzEngrgGroup]

BTW - Balax suggests 0.078 for a 75% 2-56 thread using their form taps. 0.08 will give you 55%, which should be plenty for most applications. You could even go a few thou more, to make tapping easier, and compensate for the difficult material.

http://balax.com/sites/default/files...talog-2012.pdf

Regards,
Ray L.

[J S Machine]

Good advice, thank you.

I know Emuge is another good manufacturer. I want to automate the process to remove the hand aspect completely. I know that a machine will keep it perfectly perpendicular to the work and provide a more consistent rotation then my hand does. I know that doing anything by hand, especially without being supported with a center from overhead, is asking for trouble, so I try to avoid that. Even with the center in place from above and tapping by hand, I still feel the resistance of the titanium fighting the tap, and when you can feel the tap literally twisting under the force, you know you are right on the edge of breaking it. Using a tension compression head or something like that, I could at least automate the process and it would be much faster and more consistent.

I do see the issue with the blind hole and the spindle having to stop turning in time before it gets to the bottom of the hole. I have a feeling I will probably break more than a few taps trying to get it right. Come to think of it, I'll bet that titanium nitride coating doesn't jive with the titanium. I know that you shouldn't use tools coated with AlTiN to cut aluminum because the aluminum will weld to the coating.That could be something I am facing here. Maybe I will be better off using an uncoated tap or some other type of coating that doesn't contain titanium. I'll give Balax a call tomorrow and see what they have to say about it.

[tbev]

The smallest holes I tap in titanium is a m7x.5 buy I do it with the smallest single point thread mill. I always hear people having trouble with the tapping head, from Tormach or elsewhere. I sure am glad I blew that thing off and decided to just learn how to treadmill, it's super easy, much much cheaper, I have the different sized thread mills and I can do just about anything, I can adjust the pitch, depth, etc, it's super easy. I do use a tap for 440's buy I would do it with a treadmill if I needed too. I just landed a job that will be really small threaded holes, I think something like 0.05in diameter holes. I did a lot of 440 holes in titanium, by hand, broke a lot of taps, until I found a tap that was really good, I've done a hundred holes with the same tap now and it's great. I don't know off hand what it is, I'll find out for you tomorrow if you want, it's s night and day difference. If you have to do a lot, start thread milling, you'll never look back. It's easy, cheaper and much better. Even those small holes, once you figure it out, just make sure your centered on the hole and you'll be fine, in titanium you can take small passes and they will come out perfect. I use all Tormach treadmills, countless holes in aluminum and titanium on the same treadmills, I crashed one, that's the only time I've broken one. I'll get back to you about that tap, but look into treadmills, you won't regret it.

Sent from my SM-G900V using Tapatalk

[tbev]

Blind holes don't matter to Treadmills either, another plus.

Sent from my SM-G900V using Tapatalk

[J S Machine]

I'd really like to try theeadmiling. I have never done it. I am afraid if it because I know a threadmill for a 2-56 hole will be very small and expensive. I know that would be a much better thread.

If you had to do it what kind of threadmill would you buy and where would you get it? Like suggestions on how to get started?

[tbev]

Geurig, something like that, I'll confirm tomorrow, is the name of the tap I use by hand in titanium for 440. I absolutely couldn't be happier with Tormach bits, I've bought other 2 and 3fl bits for aluminum, much more expensive ones, but I always go back to Tormach, they are killer and they are cheap. 1/8in. 1/4in, 1/2in etc. I use their treadmills too, the smallest and the largest, and one in the middle, that gives you a really big range of threads you can make. Go with the single point ones, that's all I use. I do all kind off random things with them, tonight I did a 54mm id and od pair of threads tonight, I made a visor for a scope, super easy, came out perfect. I'll help you out with anything you want to get you get started, shoot me a pm anytime. I'm assuming your running a Tormach?

Sent from my SM-G900V using Tapatalk

[J S Machine]

Yes I have a 770.

[pickled]

Ti sucks to tap. I've ran 2-56 and 4-40 here and it was an expensive learning process. The wrong coating will kill you quick because it promotes adhesion. I run uncoated taps and lots of lube. Form tap is the ticket and shoot for one drill size larger than stated in the charts for a 55% thread in steel. Did you ever read this thread over on the Blade Forums?
Tapping titanium-what am I doing wrong?

[CadRhino]

I bought a t/c tapping with my machine and only used it once. I switched to threadmill a and am happy.

I've been trying to figure out tapping titanium for some time and I have had a lot of trouble with it. Initially I was using very good YMW Japan made cutting taps and I kept breaking them. I did a lot of research and found that using form taps was the better idea and also using Castrol Moly-Dee CF cutting fluid.

I'm at a point now where I could really use the benefit of tapping in the machine but I'm not sure which way I should go. I know Tormach sells the tension compression heads but I've also had people recommend the Tapmatic heads as well. I do a lot of very small holes like 2-56 or 4-40 and they are blind holes.

Any advice would be appreciated. Breaking Taps is getting expensive. It is a weak point in my process that I have got to get nailed down.

[AUSTINMACHINING]

I'd really like to try theeadmiling. I have never done it. I am afraid if it because I know a threadmill for a 2-56 hole will be very small and expensive. I know that would be a much better thread.

If you had to do it what kind of threadmill would you buy and where would you get it? Like suggestions on how to get started?

Thread mill for sure. Low cutting forces etc. Great in blind holes. Here's a link for some I've used.

http://sct-usa.com/wp-content/upload...15_UN_SPTM.pdf

[SCzEngrgGroup]

IF you're going the threadmill 2-56 threads, I would consider a single-point threadmill a bit on the nutty side. You're talking about a tool with a cutting diameter on the order of 1/16", and a shank even smaller than that! It would be incredibly delicate, and VERY easily broken, and also incredibly slow with a 5K RPM spindle in Titanium. FAR better would be a multi-point threadmill, like this:

2-56 3 Flute 0.065 DIA Thread Mill ALTIN - End Mills - Cutting Tool - Products

It will still be delicate, but not nearly so bad as the single-point tool, and it will get the job done at least an order of magnitude faster, due to having to make only a single pass, rather than one pass per turn of thread, and the vastly greater stiffness of the tool.

Regards,
Ray L.

[CadRhino]

I buy my threadmill a from maritiitool

I'm mainly doing 2-56. Since I'm doing form taps, I'm doing the drill a formed thread calls for. It is a 5/64 (.078" or so)

[J S Machine]

I see a carbide three flute, TiAlN coated, 15 degree spiral treadmill on eBay. For about $75, I'm afraid to even buy it. Lol. I've never done any thread milling and I'm just afraid I'll break it.

[J S Machine]

Also I have a 10k spindle.

[AUSTINMACHINING]

I see a carbide three flute, TiAlN coated, 15 degree spiral treadmill on eBay. For about $75, I'm afraid to even buy it. Lol. I've never done any thread milling and I'm just afraid I'll break it.

That's why you buy 3 of them :-). I do test cuts on aluminum starting with multiple step overs to dial in the tool path, then creep up to harder materials.Pay Attn to mfr recommended cutting parameters, and you should be ok. To look at these tiny tools for the first time, I was thinking "there's no way this could work". But they do. I drilled some .006" holes .25" deep. I couldn't even see the flutes on the drill bit !. Lol. Be aware that dropping the tool can snap the shank just under its own weight (no tool holder).I've done it. "Well sh#$#", there goes 50 bucks".

[tbev]

I gotta say I didn't think it was going to work either...but I've been super amazed every time. I agree, start on aluminum, just make sure you use the coordinates for the hole, creep up on it. Ray is right, the single point tm will take a lot longer, that's just what I've always used, going to get the same ones he linked for done really small holes I have coming up.

Sent from my SM-G900V using Tapatalk