# Tapping Titanium--with an M1.6x.35 tap--any tips?



## LEDobsession (Oct 17, 2013)

Does anyone have any experience, tips, or advice for tapping 6AL-V4 titanium with a tap so small? I don't have a lot of experience with titanium as it is and I've put myself neck deep in a project that will require some very small bolts, M1.6x.35. I'll be doing it all in an Okuma Multus B300-W mill/turn 5 axis so rigidity and everything will be controlled quite well. I just thought I'd ask around to see if anyone has had any experience with this.


----------



## KC2IXE (Oct 18, 2013)

As you probably saw, I'm new to Ti, so can't help there, but I'd say check how much depth of thread you REALLY need, and drill for that. Takes a lot less effort to tap a 75% hole than a 80%. That, taps designed for Ti (coatings) and GOOD lube (not coolant)


----------



## precisionworks (Oct 18, 2013)

Will you thread mill these? Tooling is commonly available for M1.4 & larger so M1.6 shouldn't be hard to find. 

If using a conventional tap will you set up for rigid (synchronous) tapping? On 6-4 the number to shoot for is a 55%-60% thread if using a conventional tap.


----------



## Bruceter (Oct 19, 2013)

I had a friend who works in a shop who had a lot of 4-40 holes to tap in Ti. He called Balax and talked to their tech support people about the job. He ended up using a form tap with a heavy duty tapping oil (Moly-Dee I think) He was told that in the smaller sizes a form tap was stronger because of the lack of flutes. I would give Balax a call and at least see what they have to say about it.

Bruceter


----------



## LEDobsession (Oct 19, 2013)

KC2IXE said:


> As you probably saw, I'm new to Ti, so can't help there, but I'd say check how much depth of thread you REALLY need, and drill for that. Takes a lot less effort to tap a 75% hole than a 80%. That, taps designed for Ti (coatings) and GOOD lube (not coolant)



The tap drill size was a .0492" (1.25mm) and I pulled that from our tap/drill charts we have all over our shop. I think that accounts for around 65-75% thread depth, if I remember correctly. 



precisionworks said:


> Will you thread mill these? Tooling is commonly available for M1.4 & larger so M1.6 shouldn't be hard to find.
> 
> If using a conventional tap will you set up for rigid (synchronous) tapping? On 6-4 the number to shoot for is a 55%-60% thread if using a conventional tap.



I hadn't even thought of a thread mill that small. I guess I've seen them around but we don't typically have many metric taps/thread mills that small on hand, as most of them are considered "specialty tooling." I'll look into it though. If I do anything with conventional or thread forming taps it will be rigid tapping. 55-60% thread will definitely make it easier to tap than at 70-80%.

The parts that I'm making are actually a copy of an original piece of copyrighted artwork, that I have special permission to copy from the owner. I've spoken with him about the tapping and he told me, "My machinists use a special tapping chuck that will stop right before it breaks, back it off, then ratchet down again. Not sure what it's called, but it will save you a ton of money in taps and wasted parts." I don't know what a special tapping chuck would be, but it sounded like some of the old floating heads that we used in the machines that weren't equipped with rigid tapping. Do you have any idea what those might be?



Bruceter said:


> I had a friend who works in a shop who had a lot of 4-40 holes to tap in Ti. He called Balax and talked to their tech support people about the job. He ended up using a form tap with a heavy duty tapping oil (Moly-Dee I think) He was told that in the smaller sizes a form tap was stronger because of the lack of flutes. I would give Balax a call and at least see what they have to say about it.
> 
> Bruceter



That's interesting. I had our supply guy talk to our Kennemetal Rep and he told him that thread forming taps would work just fine. We use Molly Dee quite frequently at our shop, so that wouldn't be a problem. Maybe I'll just use a thread forming tap!


----------



## precisionworks (Oct 20, 2013)

LEDobsession said:


> ... "My machinists use a special tapping chuck that will stop right before it breaks, back it off, then ratchet down again.









The gold colored tap (size 4-40) is a Guhring powdered metal that works well in Ti-6-4. Tapping head is run in a mill or drill press & has a selectable clutch plus auto reverse. These are old school but a number of top shops run them in Ti as there's no chance of thread stripout (which can happen with rigid tapping). One shop owner I spoke with has a number of 5-axis machines but stills uses the tapping head for small holes in Ti.

Retail on the 30X is $718. Seems like I paid about 15% of that on eBay.


----------



## KC2IXE (Oct 22, 2013)

Got a 30x clone on craigslist a month or so back for a whopping $30


----------



## LEDobsession (Oct 24, 2013)

precisionworks said:


> The gold colored tap (size 4-40) is a Guhring powdered metal that works well in Ti-6-4. Tapping head is run in a mill or drill press & has a selectable clutch plus auto reverse. These are old school but a number of top shops run them in Ti as there's no chance of thread stripout (which can happen with rigid tapping). One shop owner I spoke with has a number of 5-axis machines but stills uses the tapping head for small holes in Ti.
> 
> Retail on the 30X is $718. Seems like I paid about 15% of that on eBay.



Hey, thanks! I'm sure that's the guy! I'll look around at work and see if we have one that small. I know I've seen one before but I'm pretty sure it was one of the bigger sized ones. I hope we have one, because I'm not spending the much on one, unless I can find it online for a steal. 



KC2IXE said:


> Got a 30x clone on craigslist a month or so back for a whopping $30


That's the deal I need!


----------



## darkzero (Oct 25, 2013)

Yup I love my Tapmatic, one of my most favorite accs I have got for the mill. Had to tap 140 blind holes a while back & took me only 2 hrs to tap em all.


----------



## precisionworks (Oct 25, 2013)

LEDobsession said:


> ... I'm not spending that much on one, unless I can find it online for a steal.



Even at $200-$300 (about the average eBay price) they can be less costly than scrapping a part that has four hours machine time already invested. Murphy's Law as applied to machining is "Everything is perfect until everything goes to hell on the final op."



> Had to tap 140 blind holes a while back & took me only 2 hrs to tap em all.


Copy that. Without the head that could take 2 days instead of 2 hours. And 10X more stress, even if you don't break that tiny tap & leave it in the part. If the tap breaks it can always be burned out with EDM but that usually costs more than the tapping head.

As always on eBay look at the photos. No photo or poor photo means either that the seller cannot take a good pic or that the head is worn out junk. There are a *few* nice used Tapmatic heads & there are also a metric ton of badly abused heads. They aren't hard to rebuild if you have patience & dis-assembly of any used head is a good idea - at the very least it may need fresh grease. 

A Tapmatic head is money well spent.


----------



## LEDobsession (Oct 26, 2013)

darkzero said:


> Yup I love my Tapmatic, one of my most favorite accs I have got for the mill. Had to tap 140 blind holes a while back & took me only 2 hrs to tap em all.



That's awesome, especially if in a manual mill!



precisionworks said:


> Even at $200-$300 (about the average eBay price) they can be less costly than scrapping a part that has four hours machine time already invested. Murphy's Law as applied to machining is "Everything is perfect until everything goes to hell on the final op."
> 
> Copy that. Without the head that could take 2 days instead of 2 hours. And 10X more stress, even if you don't break that tiny tap & leave it in the part. If the tap breaks it can always be burned out with EDM but that usually costs more than the tapping head.
> 
> ...



The more I think about it, the more I'd like to buy one, I just don't have the money for it right now. Hopefully we have one in our shop. I haven't really asked around too much, so I'll get on that. I still have a couple of weeks before I can actually get to the Multus as it's running some production right now, but it is occasionally open and just sits, so I figured I'd put it to work. 

It would definitely be worth having, being that each part is somewhere around 3 hours to run. Amen to the Murphy's Law on the last op. That is also true for the last hour of the night on the last day of the work week, no matter what part or op it is. Haha. 

Burning out a tap that small is a pain, according to our EDM department. They told me to just not break any taps. Haha.


----------



## LEDobsession (Oct 29, 2013)

Booyah! I found a tapmatic 30x in our tool room today. Now, the issue is, how do I mount it in a CNC spindle and still be able to use the little bar that juts off to the side for its tension? I thought about turning a bar that will thread into one of the coolant nozzles on the side of the spindle, but I'm not really sure about that option. What do others do that use them in their 5 axis set ups? My set up will be in a 5 axis mill turn okuma multus b300-w.


----------



## StrikerDown (Oct 29, 2013)

http://www.youtube.com/watch?v=W_tkCZgNutI


----------



## precisionworks (Oct 30, 2013)

Mine is table mounted, just like the video. These are meant for drill press or manual mill work. What you need is a Tapmatic CNC head that has the torque arm built in: http://tapmatic.com/products-page/self-reversing-cnc-tapping-attachments


----------



## LEDobsession (Nov 3, 2013)

I guess having a bar on the table would work, but I'm not sure how I could apply that setup to a lathe chuck to work with the live mill spindle.

I talked to our tooling supplier about using a roll form tap and he recommended I not use one with a blind hole, and especially not with molly dee as that would thread-lock the tap and break every one of them. I showed him the parts I'm making (my own wedding band) and he told me for my application that I should just drill to the biggest minor diameter I can with a regular fluted cutting tap, running our Hocut coolant on it. A larger minor diameter, though taking my thread percentage down to near 55%, will be easier to drill, and it's not too critical that my threads be super deep because its just to fasten one part to another, and hold it onto my finger. 

What do you guys think?


----------



## precisionworks (Nov 4, 2013)

LEDobsession said:


> ... taking my thread percentage down to near 55% ...


55% is a good number. Image below (from Tapmatic) tells the story:






All tap manufacturers show tables with 75% but that represents only a starting reference. In thin material (where you might have only 1 or 1 1/2 full threads) 85% is better. Average commercial work runs 65%-75%. Tough materials that like to eat taps can go as low as 50%.



> ... molly dee as that would thread-lock the tap ...


First time I've heard that. The go to fluid for Ti is dark sulfur-based oil when the part is not super critical (meaning medical or aero). Both those applications require non-sulfur oils.


----------



## LEDobsession (Nov 6, 2013)

precisionworks said:


> 55% is a good number. Image below (from Tapmatic) tells the story:
> 
> All tap manufacturers show tables with 75% but that represents only a starting reference. In thin material (where you might have only 1 or 1 1/2 full threads) 85% is better. Average commercial work runs 65%-75%. Tough materials that like to eat taps can go as low as 50%.
> 
> First time I've heard that. The go to fluid for Ti is dark sulfur-based oil when the part is not super critical (meaning medical or aero). Both those applications require non-sulfur oils.



When he explained how much I need the threads for this application, it made a lot of sense. I'll shoot for 55% then. 

The difference between a 50% and 55% thread depth is only .0009" ( 1.37mm is 50, 1.35mm is 55)!


He only told me that Molly Dee would cause it to thread lock in that size of a tap and being that it's a blind hole. It's not that deep of a hole (about .150," if I remember right), but at that diameter, I need to be careful.


----------



## Data (Nov 7, 2013)

I agree with what other people have said, go for shallow thread depth if you don't need too much strength. Running a thread cutting tap in titanium is always risky. 

I myself never tap titanium, I always use treadmills. The 0-80 thread mill that I use in the 007 body, has cut hundreds of holes!


Cheers
Dave


----------



## precisionworks (Nov 12, 2013)

Data said:


> ... I myself never tap titanium, I always use threadmills. The 0-80 thread mill that I use in the 007 body has cut hundreds of holes!



I see that a lot in the productions shops that do contract work for me - while the part is in the machine (meaning the datum points are known) it's faster to run a drill cycle followed by threadmill. The miracle of helical interpolation 

Quite a number of knife makers use machining centers but then drill & tap the clip mounting holes on a mill with tapping head. Probably their machines can't do helicals or they'd be machined during the shaping/contouring/drilling ops. 



> ... I hadn't even thought of a thread mill that small. I guess I've seen them around but we don't typically have many metric taps/thread mills that small on hand, as most of them are considered "specialty tooling." ...



A short article & video here: http://www.mmsonline.com/articles/thread-milling-on-a-tiny-scale

Threadmills can either cut a dedicated pitch that UN or metric:





Or they can cut a range of pitches in both UN & metric:


----------



## LEDobsession (Nov 13, 2013)

Hey, now we're talking! I knew there should be some threadmills that small. I'd love to get a few of those. They're probably upwards of $100 and they don't have any way to just get a price quote for a lowly machinist like myself.


----------



## precisionworks (Nov 14, 2013)

LEDobsession said:


> They're probably upwards of $100 ...



In size 0-80 they run about $70 & that size is a bit smaller than M1.6. The fastest way to get a quote is to phone MSC & ask them to quote some of the more common products:

Komet 88977001000005 

Kyocera 98M16-0350.4FA1 (uncoated)

Kyocera 98M16-0350L4FA1 (AlTiN coat)

Vardex D3T03012L034-I0.35ISO TM (up to 2D)

Vardex D3T03012L050-I0.35ISO TM (up to 3D)

The numbers above are stock items so delivery should be quick, normally a drop ship from the maker to you. Quite a few more available from different makers in sizes all the way down to M0.5 X 0.125


----------

