Blind Hole Form Tap Question

Pete Deal · Dec 23, 2019

I have some parts that I have been making for some time that have M3x0.5 blind holes. Material is 6061 alu, hole is about .4" deep and tapped to about .36". I want go from an H6 fit to an H4 fit so I ordered some new taps. I wanted taps with a groove to let the coolant out but could not see where they specified that. What I ordered are Balax bottoming taps. I went ahead and ordered them thinking they would not make a bottoming tap that was not meant for a blind hole right? Anyway, these don't have a groove to let the coolant out. Is this needed? Tapping at 4k rpm.

kevin66 · Dec 23, 2019

The smaller diameter taps don't seem to offer an oil groove. I have gotten them to work before but at slower speeds. The coolant/oil has to escape past the tap somehow and the quicker you get to depth the more hydraulic pressure builds up.

DavidScott · Dec 23, 2019

I tap to the absolute bottom of a .45" hole in 6061 with 10-24 Balax form taps with no problem. I also get my taps chromed which helps when tapping above 80% threads.

Pete Deal · Dec 23, 2019

Thanks guys! I did manage to squeeze a last minute call into them at the end of the day here. The guy at Balax said the same. Seems like that coolant has to squeeze out through a small space in a hurry.

David: I am only at about 65% threads now but may go a little tighter we'll see. Good to know.

gustafson · Dec 23, 2019

How are you drilling them

what size are you using.

form taps are very conditional on hole size.
I blow into aluminum with no center drill so I use a smaller than spec'ed drill to get the minor diameter down where it needs to be.

eaglemike · Dec 23, 2019

Some taps have the coolant escape built into the form of the tap, as opposed to just having straight cuts like a straight flute.
I don't think you are going to have issues. All the Balax form taps I've ever used have worked very well in 6061 or 7075 or 2219.
I have had to drill and ream at times to get the minor where I wanted it. Last few years I've been using the 3 flute carbide (150 degree point)drills and having wonderful success with them, both in feed rate and hole quality.
Good luck!

ETA: my favorite drill for aluminum are the MA Ford , series 229. IIRC it was GKoenig that told me about them. I think BrotherFrank also mentioned them. They out perform 2 flute Guhring by a bunch.

Pete Deal · Dec 23, 2019

I have been using .110 drill size but switching to 7/64 (.1094). I plan to check as I go to verify what hole size I actually have.

Eric U · Dec 23, 2019

Hi Pete...just the 2nd PM member I’ve met in person!

I run some Balax form taps in M3 and M3.5 in 6061. I think these taps have non-round profiles (square-ish). That profile allows coolant to escape. No coolant groove needed.

Mike1974 · Dec 24, 2019

Eric U said:
Hi Pete...just the 2nd PM member I’ve met in person!

I run some Balax form taps in M3 and M3.5 in 6061. I think these taps have non-round profiles (square-ish). That profile allows coolant to escape. No coolant groove needed.

Yes. Smaller form taps are not round, they are somewhat ob-round. We don't tap at that high of rpm so can't speak to that...

gustafson · Dec 24, 2019

Pete Deal said:
I have been using .110 drill size but switching to 7/64 (.1094). I plan to check as I go to verify what hole size I actually have.

This is the key, finding a process that gets you a particular size hole that you want so you get the minor diameter that you want.

Pete Deal · Dec 24, 2019

Thanks all! What I have has worked amazingly well. In fact the tap I am currently using has tapped many hundreds of holes and I think was the first tap I used in my machine and fully expected to hear a snap and see a broken tap the first time. It has been great. I just want it a little tighter.

I will spend some time drilling and tapping some scrap and checking hole size. I have also found that looking at the tapped hole under a microscope is helpful to see what is actually going on.

Mike1974 · Dec 24, 2019

Pete Deal said:
Thanks all! What I have has worked amazingly well. In fact the tap I am currently using has tapped many hundreds of holes and I think was the first tap I used in my machine and fully expected to hear a snap and see a broken tap the first time. It has been great. I just want it a little tighter.

I will spend some time drilling and tapping some scrap and checking hole size. I have also found that looking at the tapped hole under a microscope is helpful to see what is actually going on.

Awesome that it is working for you! A couple tips from a long time thread form tapper (LoL). We use modified bottoming, 2-3 thread lead, and thread to the near bottom of the full diameter. Here is my formula (I am the sole programmer so everything I do is to these numbers) -

4-40- drill +.03" from tap depth (drill .40, tap .37)
2-56- drill +.025" from tap depth (drill .30, tap .275
0-80- drill +.02" from tap depth (drill .30, tap .28)

Those are numbers for a standard 118 drill tip angle, might want to experiment if you are using 130-140deg point drills. I've not broken a tap using those numbers yet (about 14months at current job doing that). Your M3 is real close to a 4-40 (4-40 .112" - M3 .118") so I would be confident enough to use the numbers I presented. Keep in mind we use modified bottoming, so there is a bit more lead/chamfer to accommodate the very tip of the tap.

Search

Largest Manufacturing Technology Community on the Web

Search

Blind Hole Form Tap Question

Pete Deal

Titanium

kevin66

Aluminum

DavidScott

Diamond

Pete Deal

Titanium

gustafson

Diamond

eaglemike

Stainless

Pete Deal

Titanium

Eric U

Hot Rolled

Mike1974

Diamond

gustafson

Diamond

Pete Deal

Titanium

Mike1974

Diamond

Similar threads