[MFchief]

Hi All,

I am planning to acquire some thread forming taps to give them a try. They seem to have a good reputation here on the board.

But looking over the available taps got me thinking. So, since I am talking about using them in my Tormach with a Procunier tapping head, is there a reason not to buy bottoming taps? I'm thinking that we have good control of the tap for starting the thread so no need for the "taper" function of a plug tap, and the bottoming tap would yield slightly deeper threads on a hole that was not a thru hole.

Is this logic flawed? Advice would be appreciated.

Terry

[soymilk]

I've become a big fan of threadmill. I've talked to people that threadform and they are generally pretty happy until the tap breaks. With threadmills, I like the fact we can generally replace the tool, touch off the offset and recut the thread no problem.

I love emuge taps. We were able to get into the 1000's with emuge. Granted we are only tapping .4 deep into nitronic 60 with an emuge 10-32 tap

[SCzEngrgGroup]

Plug taps take more torque to turn in, due to the shorter taper. They're effectively taking a deeper chipload. This will likely lead to shorter life, and more frequent breakage.

Regards,
Ray L.

[R.DesJardin]

I use thread forming taps quite a bit and I buy the bottom taps, they seem to work just fine power tapping on the Tormach. It's nice not to have chips getting in the way.

[rcs60]

bottom taps are good for most threading application the times that i used plug taps is when the material is a little bit tough to machine like 4140 heat treated to 32 rc
it really comes down to if the material flows ok use a bottom if it flows harder use a plug
when the material is harder use a cobalt tap with a coating to improve the number of tapped holes per tap

[MFchief]

Thanks all for you comments. I do use thread milling on the Tormach, but for me at least, if there are a lot of holes to thread, tapping is quicker. I think if I do use the forming taps it would be about 90% in aluminum. Since the forming taps are pretty pricey, I was hoping that just buying the bottoming taps would save money and cover more situations.

Terry

[Don Clement]

I have done extensive tapping of blind holes in 6061-T6 ( 10s of thousands) with my Tormach using a Procunier 1E tapping head. I use forming taps because there are no chips formed and don't have to expel chips out from a blind hole. With the Procunier 1E the maximum size recommended forming tap in aluminum is a #8 http://www.rockford-ettco.com/Downlo...1000-13000.pdf and the maximum cutting tap size is 1/4 or M6. Anything above a 1/4" I threadmill. I use forming taps for anything less than #8 and spiral flute cutting taps for tapping blind holes for 1/4 and M6. For #10, in spite of Procunier's recommendation, I sometimes use either forming or cutting taps. The two spiral flute cutting taps shown below are 1/4-20 and M6. The chips are expelled out the top of a blind hole using a spiral flute cutting tap. BTW the Procunier is perfect for blind holes as it stops within 1/3 revolution. Programming the Procunier is simple and straight forward: Feed is at 100%, no dwell, and retract at 200%

Don Clement

[Hirudin]

I'm a fan of thread forming taps and I have been using the bottoming type almost exclusively. So far they seem to work very well. I haven't had one break on me though, when one does I imagine my opinion might change, as soymilk suggested. When I need to use a cutting tap I usually go straight to bottoming as well.

I think the biggest difference between the different types is how many "teeth" are actually cutting/forming the thread. With a bottoming tap, only a couple teeth are making the thread whereas with a tapered tap the load is spread out between several teeth. I bet the biggest consequence might be tap life. Personally, although they aren't "cheap" they're "cheap enough" that the idea of the lifespan being diminished doesn't bother me.

If you haven't already seen it, check out the video below. I haven't seen it in a while, but I think the question of "well why don't I just use a bottoming tap all the time" is asked and answered. I think I'll go watch it again as well.
https://www.youtube.com/watch?v=kcVaKofymqU

[Don Clement]

Perhaps why I am successful in using bottoming forming taps on blind holes is because I start with a spot drill down low enough to create a countersink with enough room for clearance of the forged material from the forming tap. This also makes for a countersunk guiding opening for the bottom tap.

Don Clement

[Mazaholic]

coolant coolant coolant.I can't stress that enough.especially when taping aluminum . That's one of the main problems when using thread forming. Plenty of coolant is a must.
Once you are sure you have enough coolant in the right concentration,then you can estimate tool life thru trial and error.
You should get about the same amount of parts for each tap during a run with the right coolant.
Forming taps are pretty consistent as far as tool life but thread forming creates a lot of heat....again...coolant.

[Don Clement]

I use Relton A9 when form tapping in aluminum and no coolant. Metal Cutting Fluids - RELTON PNT-A9 Aluminum Cutting and Drilling Fluid, Pint - Mo Clamp, Simpson Strong-Tie, QuikDrive, Reelcraft, Fomo Foam - FastoolNow.com

[MFchief]

I liked the video, not too much new info, but he did a good job presenting it. His comments about the wear on the first few threads of the bottoming taps made sense, but made me wonder if you could renew them by grinding off the first couple and the reforming the slight taper?

Don, I know you do a ton of tapping, have you got a feel for how many holes you can tap with a bottoming tap before it starts to show wear? I've got a feeling you tap more holes in a month than I have in my life!

Terry

[Don Clement]

Don, I know you do a ton of tapping, have you got a feel for how many holes you can tap with a bottoming tap before it starts to show wear? I've got a feeling you tap more holes in a month than I have in my life!

Terry

I use Balax forming taps and haven't got a quantitative feel other than in 6061-T6 with Relton A9 the Balax form taps last a very long time.

[Mazaholic]

Don,if i tried to use the Relton,i'd pull back a tap with a glob of aluminum on the end. We tap 3 - 4,000 rpm with a 6mm tap using a 1,000 psi thru tool coolant system.
My point was,once you have the proper coolant (or lubricant) form taping is the way to go up until the H/P of the machine is reached.
You can bet the tap life will be consistent + or - 100 parts.
Bonus advantage is that formed threads are a lot stronger than cut threads.
Balax,OSG,and Titex are some very good brands.

[MFchief]

Thanks again guys, based on what Don and Mazaholic are saying, I don't believe rapid wear out will be a factor for me with my tapping rate. I'm going to order some Balax taps and start playing. LOL

Terry

[Don Clement]

Don,if i tried to use the Relton,i'd pull back a tap with a glob of aluminum on the end. We tap 3 - 4,000 rpm with a 6mm tap using a 1,000 psi thru tool coolant system.
My point was,once you have the proper coolant (or lubricant) form taping is the way to go up until the H/P of the machine is reached.
You can bet the tap life will be consistent + or - 100 parts.
Bonus advantage is that formed threads are a lot stronger than cut threads.
Balax,OSG,and Titex are some very good brands.

Really you are using a thru tool coolant on a 6mm tap your Tormach @4K rpm. I use a Procunier 1E on my Tormach with a maximum of ~1K rpm . BTW 6mm forming tap is too large for the Procunier 1E. Relton A9 works very good with my setup on a Tormach for blind holes. I use a spiral flute cutting tap for 6mm with Relton A9. For larger than 6mm or 1/4" I threadmill no thru the tool coolant needed.YMMV

[Mazaholic]

No we have Makino A64NX and an OKK HMC500. I just responded because I was giving credits to thread forming over cutting. Not really machine specific.
Thread forming is the best choice for any machine.The only draw back is wall thickness of the hole. Some holes are too close to the wall of a part and it just doesn't work.

[CadRhino]

I have been threadmilling quote a bit up yo 5/8" but mostly #6-8 and only use koolmist coolant as the lube. Haven't had any issues yet.

Really you are using a thru tool coolant on a 6mm tap your Tormach @4K rpm. I use a Procunier 1E on my Tormach with a maximum of ~1K rpm . BTW 6mm forming tap is too large for the Procunier 1E. Relton A9 works very good with my setup on a Tormach for blind holes. I use a spiral flute cutting tap for 6mm with Relton A9. For larger than 6mm or 1/4" I threadmill no thru the tool coolant needed.YMMV