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...

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 (http://www.tapmatic.com/) 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.

:cheers:

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.

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

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! :D Best check this out before you drill all the holes too large.

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

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

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.

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... :)

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

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.

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.

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)

fpworks

These taps are not carbide they are powdered metal coated in TIN. Keep in mind you must have high rpm for the TIN to work. We are doing the machining on a Brother TC-22A VMC. Thread gage and ID pin gage still the same as the first hole. The tap drill is a Gurring HSS 7.3mm parabolic drill uncoated and needs resarp after about 5,000 holes. Flood coolent with Blazer cut swiss lube at 7.0 on the refact.

Go to www.lmtfette.com

solgood,
Let me get this into my brain. You're tapping 5/16"-18 @ 8000 RPM? In 6061, Derlin, wrought iron, cast, uranium, titanium, butter, LP-410 6/6, dirt, Inconnel 625, 304 2B, 15-5ph or air.
How do you get the 444.44444444444444444444444444 inches per minute feed required to do this?
Karl

Karl

If you were to read carefuly you would notice that im talking about 6061T6. I have no prob. getting the feed to do such tapping. The machine is able to do a max of 8000 RPM in tapping.

solgood,
Let me get this into my brain. You're tapping 5/16"-18 @ 8000 RPM? In 6061, Derlin, wrought iron, cast, uranium, titanium, butter, LP-410 6/6, dirt, Inconnel 625, 304 2B, 15-5ph or air.
How do you get the 444.44444444444444444444444444 inches per minute feed required to do this?
Karl


We also have a machine capable of 10,000 rpm and 1600 ipm feed however, do to exceleration and deceleration the thread would have to be fairly long to get up to speed before reversing and backing out in a sycronis tapping cycle. It is possible though. :D

A.J.L.

Something I've wondered about rigid tapping: is the synchro sophisticated enough that the feedrate ramps up as the spindle speed ramps up in true electronic cam type mode, or is it more just a 'throw the switch and hope she makes it' kind of deal?

Reason I ask, my 96 Haas has open loop spindle which means the control really has no way of producing a simultaneous move with the spindle, yet it seems to track the thread path very accurately. Why does the tap not have trouble at the bottom of the thread as the spindle slows down and stops, then ramps back up on the way out?

Something I've wondered about rigid tapping: is the synchro sophisticated enough that the feedrate ramps up as the spindle speed ramps up in true electronic cam type mode, or is it more just a 'throw the switch and hope she makes it' kind of deal?

Reason I ask, my 96 Haas has open loop spindle which means the control really has no way of producing a simultaneous move with the spindle, yet it seems to track the thread path very accurately. Why does the tap not have trouble at the bottom of the thread as the spindle slows down and stops, then ramps back up on the way out?

You answered your own question Hu. If it is possible to tap in, stop and reverse out the machine must be sophisticated enough to ramp the feed with the spindle acceleration. Not only that with repeat rigid tapping you can do it several times on the same hole.

edit:
Open loop means the spindle speed is not tightly controlled but that does not mean the controller does not know accurately how fast the spindle is going. Yes????

...not to be a smarta$$ but i can't help myself.

How to tap 1000 2-56 holes in Aluminum?

~~~One at a time, very carefully!

:D I love that one...

As for rigid tapping at higher speeds, I'm doing it at 700 rpm because a colleague mentioned that with older machines (like my 94 Mazak) that he wouldn't risk going beyond that, though I don't really remember why... maybe backlash, or synchronicity or something...

But I think once I'm done this job, I'll have to take a block of aluminum and crank it up a bit and see what happens.

So question: with rigid tapping, do you need to leave some lead in space for the spindle and feed to synchronize, or can you rapid your tap right to the whole entrance and start from there?

A 2-56 thread job you should rapid 0.250 below the start of the hole. Make sure the boss is watching the first one.

Just kidding.

I guess it all depends on the machine & control. But I've never heard of anyone rapid traverse to the surface then tap. I'd at least expect to see some clearance for the position/servo loops to stabilize. You'd get much more consistant results, tweek from there for perfection.

As for rigid tapping at higher speeds, I'm doing it at 700 rpm because a colleague mentioned that with older machines (like my 94 Mazak)

A '94 Mazak what? I've got a '93 Mazak and I tap at 5000 rpms all day. As a matter of fact, I have quite a few from that era that can still tap at and easy 3000+ rpms all day. Maybe its something more about the machine condition? or just being "cautious".

With rigid tapping (or "synchronous tapping") you could start your tap from "zero". But its better practice to start from above the part some. Many people will start from .200 or .250 above the hole. This has more to do with reaching a particular tapping speed before entering the hole, not for "waiting for the spindle to synchronize". The spindle is synchronized from the moment the rigid cycle is turned on. Otherwise, every machine would break a tap at the start or when reversing.

Let me get this into my brain. You're tapping 5/16"-18 @ 8000 RPM?

As AJL said, "it is possible". Some machines can tap at extremely high rpms. You should see a 1/2-13 @ 10,000 rpms!!!

I still say a CNC Tapmatic is the way to go, especially for that many holes. But it might be expensive for some. Rigid tap will work.... just takes a lot longer.....

:cheers:

Thanks psychomill

I think some of these guys or gals are afraid of using there synchro tapping machines to there fullest. If the machine is old you may have too much backlash in the Z to tap at 5000 to 10000 RPM. The machine I discribed is a 2002 Brother TC-22A VMC. I start my feed at .15 above the part, but like you said it not needed.

solgood,
Sorry obout my ignorance, Ive never been around a macine that was capable of it.
Karl

Karl

No offence taken, we all work with dif. machines and dif. parts. We can all learn from each other, great to hear from you and all on the Zone.

This if for all you Machinists

Yes, we do have an extensive array of state of the art, high tech, computerized machinery, but as anyone who has ever cut chips will tell you, "the machine is only as good as the person behind the wheel!" :cheers:

I wont take credit for the quote its from a good friend.

Chad

Chad, Karl..... and others....:cheers:

"Ignorance" is the first step in learning and understanding. Otherwise, we'd all be "know it alls" right?

I think some of these guys or gals are afraid of using there synchro tapping machines to there fullest

There's some truth to that. Many could debate on the affects of "high speed tapping" to a machine. I've heard everything from early wear on the guides (linear or box) to stretching out the ball screw. I've been rigid tapping from 3000 to 10000 rpms for many years. I've never seen either happen on hundreds of machines I've programmed. The only misfortunes I've seen from tapping is when some operator fat fingers a tool length or a Z depth, uses wrong sized drill, incorrect feed, etc.

Taps can and do break. Depends on your set up, material, coolant, quality of the drilled hole, tap type and speeds. In the case of aluminum, I've found that more speed is better. Powdered metal taps work well. The TiN coat does fine in aluminum. It's not as bad as say TiCN or something which works with heat. But I've used uncoated as well at those speeds.

Since 1000 holes is quite a "few", if you only have to do one plate, being somewhat "conservative" is probably wise. But in production, I say "hit the button..... its pucker time".

:cheers:

OMG 1/2-13 at 10k!!! Form or cutting? I would pay a dollar to see that!! I usually don't go over 500rpm lol call me a baby :)

Many could debate on the affects of "high speed tapping" to a machine. I've heard everything from early wear on the guides (linear or box) to stretching out the ball screw. :cheers:


I agree, I've never witnessed any abnormal wear etc. from sync. tapping and have been doing it for years. Since the feed and the spindle "ramp up" (and down) it's no different than anything else the machine does under normal conditions. Since we'er on the thrd. cutting thing, who all thrd. mills larger size thrd's? It's a viable opption where horspower is at a premium.

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...

Use thread mill. If a thread mill breaks, your can remove the broken part of tool without problem. The programmation is just a little bit more difficult.

OMG 1/2-13 at 10k!!! Form or cutting? I would pay a dollar to see that!!

And worth every cent! :cool: Form or cutting.... I've done both.

It definately looks wicked. For the most part though, I don't program it to run at that speed. If the part only has 3 or 4 holes to tap, you don't gain much for a 1/2-13 at 10k. My only point is that there are machines that can do it. Keep in mind, the spindle has to synchronize and make the speed. Its a little different than just simply programming a G1 move to go 769.23 IPM. Many machines have the acceleration to make that feed in a very short distance of travel. But the same machine won't make it to top speed in the distance of a thread. However, if you program a 4-40 or 6-32 at that speed, now you might make a difference.

Also keep in mind of cutting forces, which brings up the next comment on thread milling. Many machines at a conservative speed, say a couple hundred RPMs can tap a 3/4-10 thread. But the same machine might not be be able to tap it at 2000 RPM. The momentary spike in force at tool entry make cause the spindle to overload. In these cases, thread milling is an option to pick up cycle time. I acually thread mill quite a few threads large and small diameter. My reason has more to do with dedicated tool magazine issues though and not horse power. But the taps I do have in the magazine all run at what most would consider "fast"....

:cheers:

We generaly don't thrd mill as a rule on production jobs. When we do it's because we have some thrd. size like 2.5" - 6" that is a one piece job and dosn't justify buing a new tap and holder when we can just thrd. mill it. I've used single point tools from the CNC lathes. We have to do this when we don't have the correct pitch thrd. insert. It's usually a slow deal in hard steel not as bad in iron or alum. though.

We generaly don't thrd mill as a rule on production jobs. When we do it's because we have some thrd. size like 2.5" - 6" that is a one piece job and dosn't justify buing a new tap and holder when we can just thrd. mill it. I've used single point tools from the CNC lathes. We have to do this when we don't have the correct pitch thrd. insert. It's usually a slow deal in hard steel not as bad in iron or alum. though.

I understand your opinion.
The tool path for threading is very long to programm. It's a pity that any CN don't have thread cycle.
I have a positive case when threading tool is better. A very expensive part with a lot holes to thread. It's impossible to have a tap broken in the part due to the cost. The workshop have a CAD/CAM and it's very easy to programm the threading of hole. If a thread mill breaks, you remove the broken part, you change the thread mill and you repeat your programm.

But if I should make a lot of part with few hole to thread, I would choose thread former. The advantage: The material around the thread is work-hardened and you don't loose time !!!!

The tool path for threading is very long to programm.


It's not so long to program. It can be a lot of cutting if you single point thread with a lathe type tool (i.e. the lathe's tool is fairly fragile, not for intrupted cutting) but still cheeper for a one off run.