[dalianharley]

Hi,

I have to tap 3 3mm holes at 5mm deep. I heard that you need to use "form tapping" for small holes. I do have 3mm HSS hand taps, will that work? This will be a small production run, at a few hundreds of these 3mm tapped holes.

thanks

Daz

[dalianharley]

to make it worse, it's blind hole...
Should I drill deeper than 5mm?

Hi,

I have to tap 3 3mm holes at 5mm deep. I heard that you need to use "form tapping" for small holes. I do have 3mm HSS hand taps, will that work? This will be a small production run, at a few hundreds of these 3mm tapped holes.

thanks

Daz

[mioduz]

What are you tapping into? Note that you need to use a larger tap drill if using a form tap. Thread milling is likely the best option for a blind hole. But that's a lot of black magic if you have never done it before

Sent from my VS980 4G using Tapatalk

[dalianharley]

it'd be 6061 alum
it's not a very stressful part, just to hold a plastic guard.
Thread milling...geez more stuff to learn

What are you tapping into? Note that you need to use a larger tap drill if using a form tap. Thread milling is likely the best option for a blind hole. But that's a lot of black magic if you have never done it before

Sent from my VS980 4G using Tapatalk

[mioduz]

Tapping AL can be finicky. It can be gummy on the finer threads. Personally I'd thread mill it but that's going to cost you buying thread Mills and likely wrecking one in the process. Prepare for likely the most costly tool you'll ever buy dollars/pound. Once you get all your settings right you'll wonder why you ever bought a tap in the first place. Getting there though may test your religion.

Sent from my VS980 4G using Tapatalk

[victorofga]

if youre not prohibited, and workpiece let you, then drill it at least 11 mm deep

even its several hundred, still worth to tapping by hand,, not with a simple crank but a tapping guide..
see picture..

actually for this short thread you could make some simple taping stuff..
even some woodframe with a bushing could hold the tap.. it just a few mm travel..

what is important sure it working easy so you feel the tap were tighting up..

picture is just an example.. a lot simpler you can make..i think you can tap around 70-100 in an hour with a guide

[Hirudin]

A thread-mill that can do a 3 mm hole would be miniscule! Personally, I wouldn't recommend trying it. I'm sure it can be done, but if you're doing a few hundred holes you'd probably want something faster too.

I've tapped several* M3 holes with a forming tap using a Procunier tapping head. I pre drill with a 2.75 mm drill to a depth 0.5 mm deeper than I plan to thread (at full diameter - the bottom point of the hole is probably about 0.65 mm deeper). The tap turns black from oxidizing aluminum so I try to hit it with compressed air to clean it off quickly between holes.

The Procunier is very expensive, but it works well and is very fast. There are cheaper tapping heads available, but the majority that I've seen have a clutch adjustment that is, as I understand it, basically done by 'feel'. That kind of guesswork doesn't appeal to me, which is a big reason I went with Procunier.

Here's a video I think you may find useful if you're considering a tapping head...
https://www.youtube.com/watch?v=IIv8xH9razE

This also looks like a very cool and versatile machine...
https://www.youtube.com/watch?v=FZLU-F9wcS0
If I remember right: at least one Flexarm model is basically the same price as a Procunier Tru-Tap head, but it looks like it would be more versatile, albeit slower. As you said: more to learn.

* maybe 30 or so - not a ton, but enough to be confident that the process I'm using works OK

[SCzEngrgGroup]

Hi,

I have to tap 3 3mm holes at 5mm deep. I heard that you need to use "form tapping" for small holes. I do have 3mm HSS hand taps, will that work? This will be a small production run, at a few hundreds of these 3mm tapped holes.

thanks

Daz

The answer to your question depends a whole lot on HOW you intend to do the tapping. Are you using a reversing tapping head, or a tension/compression holder?

In general, standard hand taps, i.e. "plug" taps, should not be used for machine tapping. They are likely to get clogged with chips, bind, and break. Spiral point, spiral flute, or form taps are recommended. Threadmilling is an option, but not a very good one for such a small size. Remember a tap is tapered, so if you need 5mm of useable threads, you'll have to run the tap quite a bit deeper (probably almost 2X). Or, you can machine tap, then use a bottoming tap and chase the thread by hand to remove the taper from the lower threads. Also, since you don;t have a servo spindle, you need to drill the hole extra deep, to make sure the tap can't bottom out (which WILL break it). Further, spiral point taps push the chips ahead of them, so you have to also allow extra room for the chips.

My recommendation would be a reversing rapping head, as it gives you pretty good control over depth, assuming your spindle speed is accurately known. I would use a spiral point tap, and drill the hole at least 3X as deep as the threads you need, and run the tap in 2X as deep as you need. Use lots of tapping lube, and blow the chips off the tap between holes.

If that all sounds too complicated or expensive, spend about $80 for a "hand-tapping fixture", and just do them by hand. It's quick, easy, and relatively fool-proof. Not as fast as CNC, but you'll probably get it done without any broken tools and scrapped work.

Regards,
Ray L.

[mioduz]

looks like most manufacturers stop at M4 on thread mills so you will have to use some kind of conventional tapping technique. Im sorry for sidetracking the topic with a technique thats not applicable here. Surely you could probably find someone to make you one custom, god knows the price and it would be incredibly delicate. I HATE tapping blind holes, and I do it for work many times a week.

[hjl4]

Spiral flute taps used with a reversing tapping head would push/pull the chips out of the hole. My experience with small taps is somewhat limited, I rarely see anything smaller then 6-32. I adjust the clutch on the Tap-Matic head to avoid breakage on blind holes. It also works great in a drill press provided you can spin it slow enough, and if you hit bottom, you just release the handle and out it goes. Definitely clean the tap between holes and ad cutting fluid such as A-1 before attempting to tap the next hole.

[redridertwo]

i would use a roll forming tap they work awesome just make sure you use the right drill size you will do all 100 holes with one tap use cutting oil on ever hole

[Hirudin]

Spiral flute taps are cool too, for sure. Below is (basically) my first foray into machine tapping. This is a spiral flute tap, as you can see: it works quite well. Now I only use forming taps because I like that they're likely stronger, likely produce stronger threads, and because it's nice that they don't produce chips.
https://www.youtube.com/watch?v=VGhm96ntPAY

[LRF]

Daz,
How many of these parts do you have to make? That information can help in the decision on which way to proceed.

[dalianharley]

Daz,
How many of these parts do you have to make? That information can help in the decision on which way to proceed.

First 12 of them, 4 identical part with 3 holes each. Then maybe a small run of 20 sets, that's 240 holes. I'm gonna try spiral and form tap see which one I like better. You guys are awesome, better than any book I bought lol. Power to the collective wisdom.

[Don Clement]

I have tapped 10's of thousands of blind 4-40 holes 1/4" deep in 6061-T6 on my Tormach using a Balax form tap and Procunier reversing tapping head. BTW #4 screw is approx 3mm. Tormach Procunier Tapping Video by miltons_stuff | Photobucket Haven't tried threadmilling a blind hole that small because the form tap and Procunier have worked so well.

Don Clement

[dalianharley]

oh man that looks gnarly. I got the tormach compression tap head and this will be the first job for it!
I'll follow up after I give it a try. Now i have to source a 2.8mm drill. any recommendation on where to source them?

I have tapped 10's of thousands of blind 4-40 holes 1/4" deep in 6061-T6 on my Tormach using a Balax form tap and Procunier reversing tapping head. BTW #4 screw is approx 3mm. Tormach Procunier Tapping Video by miltons_stuff | Photobucket Haven't tried threadmilling a blind hole that small because the form tap and Procunier have worked so well.

Don Clement

[SCzEngrgGroup]

oh man that looks gnarly. I got the tormach compression tap head and this will be the first job for it!
I'll follow up after I give it a try. Now i have to source a 2.8mm drill. any recommendation on where to source them?

Just use the closest Imperial drill - 0.110 =>7/64, #35 or #34.

Regards,
Ray L.

[Hirudin]

oh man that looks gnarly. I got the tormach compression tap head and this will be the first job for it!
I'll follow up after I give it a try. Now i have to source a 2.8mm drill. any recommendation on where to source them?

GUHRING 2 8mm 0 1102" Solid Carbide Drill Series 730 High Performance | eBay

I bought a whole bunch of drills from this seller...
zorotools on eBay
But they don't seem to have any 2.8 mm drills at the moment.
Here's a 2.75, which is the size I use for M3 forming taps.
GUHRING 9005490027500 Jobber Drill List 549 Metric Size 2 75 | eBay

And, this may be helpful...
Tap Drill Calculator

[Don Clement]

The Procunier reversing tap head is perfect for blind holes as it stops within 1/3 revolution. Can't say how a compression tap head works on blind holes.

Don Clement

[Hirudin]

dalianharley, if you decide to get a Procunier, and if you decide to buy a new one, I'd suggest buying it direct from Procunier. Call them up and have them install a quick change spindle for you - I believe this is a free upgrade. The only downside that I'm aware of with the quick change spindle is that the collets are more expensive. The quick change collets are ~$50 each instead of ~$30 each if I remember correctly. For the 15000 series Tru-Tap head (which is what is shown in the last video I posted) you're only likely to need 4 collets* so they'll cost ~$200 instead of ~$120.

Don Clement, you're a fan of the quick change collets too, right?

* what I would call a "complete set" of collets...
58811 - #6 Pro-Quick collet
58818 - #8 Pro-Quick collet
58824 - #10 Pro-Quick collet
58838 - 1/4 Pro-Quick collet