4-40 Roll form tapping - speeds?

[colton_m]

Hello,

I have some aluminum (6061) parts that require 4-40 threads (.300" deep)

I have never used form taps before but thought this might be a great project to try them out on.

I was wondering if anyone with experience running these taps could chime in with some real-world cutting parameters to try out first?

Thread: 4-40 .300" deep, blind hole in 6061
Tap: Nachi (#97784) HSSE-V with a DLC coating.
Holder: ER-16 Tap collet
Machine: 2015 Haas, has rigid tapping.

The coolant in this machine is sitting at about 10% concentration, I'd prefer to just use coolant.

The Nachi catalog suggests drilling #39 (0.0995") and running 100SFM (3570rpm).

Any suggestions would be great.

Thanks!

 

[Atomkinder]

As fast as you trust the machine

We were just running some M12x1 cut holes in aluminum at ~1800RPM. Worked fine. I would be more concerned with such a shallow hole in that the spindle won't reach 3k anyway, so maybe try 1200, then keep bumping it up until you don't see any time savings.

FWIW I love form taps.

Edit: This was in a 2012 Haas VF-6SS. Also you'll save a bit of time by setting the spindle speed but NOT using M3. The control will do it in the tapping macro and won't have to stop the spindle to orient.

 

[Evenglischatiest]

3570 RPM gives you 89.25 inches per minute. Assuming a .05" return height, that would ideally come to just under a quarter of a second to get to the bottom of the hole. And then it has to come to a full stop before the bottom. That leaves less than an eighth of a second to reach top speed. I can't imagine any normal mill spinning up that fast. I think you'd be doing incredible if you topped out at half that RPM. Even then, you end up with an average speed well below 1,000 RPM.

I program pretty much every tap (within reason) at 30 inches per minute, and match the RPM to that. I get the feeling most people program them faster, but I've never noticed their machines actually running any faster.

That said, the acceleration curves on the spindle and Z motors shouldn't let you go any faster than they can handle. If it's a new, tight machine, I say program it to the numbers Nachi gave you. But expect something closer to 2 seconds per hole. Whatever it comes out to will be the best your mill can do.

 

[Mike1974]

I just finished a job that I was using a 4-40 sti tap. I was running 1200 rpm and a feed of 30, not a blind hole however. Like some other people pointed out, the machine probably won't get to 3000+ rpm in that short of a distance anyways. I actually only am doing 5 holes per part, but my time savings between feeding at 15 and 600rpm and 30 and 1200rpm was probably 1-2 seconds (maybe...), IIRC. I know it was not much at all so its not much time savings.. By the way, this was in a Haas UMC-750 with rigid tapping, also about 10% coolant. Oh yeah, remember to check your drilled hole size! If you look up a chart with form taps, your thread percentage changes significantly for each .001 of drilled hole size, so you need your drill to cut right to size.

 

[Mike1974]

BTW, with a blind hole, a form tap is your best bet.

 

[Dave Rocks]

Run per the manufacture, in a test part, and see how it performs. One suggestion is to start your cycle above the part so you can be sure to have a nice engagement. I'd suggest .2 above the hole. Coolant will be totally fine in aluminum. I've had to use moly dee only in hardened stainless. Once you form tap, you will never want to go back to cut taps again

 

[Larry Dickman]

How many holes do you need to do? I worked at a place a few years back, every part we made had about 100, 2-56 blind holes. So that was several thousand tapped holes per day. We found it was faster to use a tapping head. Since your spindle doesn't have to stop and revverse, you can run it at 5k rpm and tap a mountain of holes in no time. It's also a hell of a lot easier on the machine.

 

[Whysosharp]

We tap 4-40's on our Hardinge/Bridgeport 480x APC at 2400 rpm and 60ipm. That's in a .625 blind hole with thread depth .55. I think whatever was recommended should be ok in my opinion.