How to tap 1000 2-56 holes in Aluminum?

[Driftwood]

Hello all...

I need to tap about a thousand 2-56 holes in several aluminum parts, blind holes, 1/4" deep. I'm a little new to this all, so I wanted to run this by you all for a second opinion.

I can't scrap any parts, so I can't break any taps. If that means going with a slightly less complete thread, then we'll take it. I planned on going with a roll form tap and drilling with a 2mm drill, catalog tells me that should still give me 60% thread. Maybe I should go bigger?

As for speed, i was thinking around 600 rpm on my vertical machining centre with rigid tapping. Its an older machine, so I don't want to push it.

Hows that sound? Any suggestions? Should I use tapping fluid?

Thanks in advance...

[psychomill]

What machine and how old? How many parts? Is it 1000 all together or 1000 per part?

2mm will be fine (I use 5/64) and roll tapping will be preferred. 600 rpm is very conservative and will take you a long, long,..... long time. But it will work. In aluminum, just be sure to use tons of coolant, and check for chips in the holes from drilling. On parts like these, I use a Tapmatic for a CNC. Goes way faster, you can tool change it, and tap up to 5000 rpms. With the self reversing head, you can program it in a bore cycle (or long hand... depends on the method)..... saves on time for the machine spindle having to reverse.

[ajl6549]

I would use a spring loaded driver even though your rigid tapping, esp. if your mach is older, as a safety precaution. Also if your machine is capable, I'd use about 3000 rpm this approximatly 75 sfm, still slow but most machines can't get up to speed in that short of distance any way. And on the tapping short and (I assume) hand tapping to depth thing, thats a lot of holes to hand tap, tap right to depth just clean chips well after drilling.

[fpworks]

I hate tapping little holes in gummy aluminum. Maybe a recent experience of mine will help:

I've been running a job that required a lot of M3x0.5 holes in 6061-T6511. I had some problems, not breaking taps, but galling up taps and ripping out threads. I dealt with Balax, and had some special taps made, and made some process adjustments:

form taps
hard chrome coating ++
4 coolant grooves ++
4H thread tolerance/limit
2.78mm hole-65% (gaged)

also, I ran my synthetic coolant at about 8-9%, and had to keep spindle speed no higher than 1000rpm, 2000rpm would instantly gall the tap. It took a while to work to the above parameters, sometimes I would get 100 holes before the tap would gall and scrap a part.

Heat is your enemy, so think about everything that will build heat.

Justin

[HuFlungDung]

If you need threads all the way to the bottom, I would use a cut thread tap. You would want to avoid retapping the holes by hand to get to the bottom! Best check this out before you drill all the holes too large.

I'd vote for the reversing tapping head idea on this, too.

[lakeside]

Originally Posted by HuFlungDung If you need threads all the way to the bottom, I'd vote for the reversing tapping head idea on this, too.

I'd use a roll form form 2-56 bottom hole and a Ridged holder

[solgood]

You should have no prob. I have found that Fette makes the best form taps, dont go too slow because the TIN on them needs heat to lubricate. Use a solid holder with a tap collet for your tap size. Start your feed at .15 above the part. No need for tap lube unless you have synthetic coolent. Use a 90 deg. stot drill so your thread doesnt stick out above the surface and its easyer on the tap. Do not try to use a cutting tap 6061 forms like a dream.

[Driftwood]

Thanks for the reassurance guys.

I'm about half way through the holes and so far so good. I don't have a collet tap, just regular ER-16, but it seems fine for such small taps. Not using any cutting fluid, just lots of coolant.

Wish me luck... don't want to be here on the weekend...

[brent1]

rigid tap using form tap if your machine cam rigid tap it is knew enough to
bump up rpm try 2000

[fpworks]

solgood,
I disagree with using any TiN coated tool in aluminum, especially taps and drills, and especially form taps. Aluminum has a tendency to stick to the TiN coating, so bright (uncoated) tools are a better choice over TiN for aluminum workpieces.

[solgood]

fpworks

I would agree with you for most form taps, but you must try the Fette line of form taps. I have taped 4-40 thru 5/16-18 in 6061 at 8000 rpm with no prob. I curently have a 5/16-18 Fette that has more than 300,000 holes to its name, 1.5" deep blind, 7.3mm tap drill. The treads look great and the tap looks like it just came out of the box.

[fpworks]

solgood,
If that is the case, I'm going to buy some next week!

That kind of tap life is unheard of, but I can accept that there are advances in tooling that make what was impossible now possible. May I assume that you are gaging the threads as well? Is this a carbide tap?

Seriously, I will buy one next week (as long as it is not a carbide tap...too pricey for most cases)