Life od a thread forming tap.

[graemeian]

Like many, I use form taps in my milling center because there are no chips to break small taps. I was wandering just how much 6061 Aluminum will a form tap make. I have a CNC job that will require 1000s of 4-40 tapped threads in 6061. Would a Balax or OSG tap go 200 inches without reducing the thread size noticeably? That would be 800 1/4" deep holes. Tapping speed would be 2000 RPM. Thanks.

Similar Threads:

• Thread forming vs thread cutting in plastic
• Thread forming Taps
• Thread forming
• Thread Forming Aluminum
• Thread Forming

[rcs60]

i just finished tapping 6-32 x 3/16 deep the tap went through about 5000 holes in steel the tap was still good this was on a robodrill at 4000 rpm and 125 ipm feed
on our swiss machines the taps (10-24) are run 800 rpm with a floating holder has gone through 50,000 holes in 6262t6 material
the best tool life i found was to use a good brand tap that is listed as cobalt as the base material

[graemeian]

Wow, that is a lot of use on a tap. I do have an 8-32 form tap in my machine that I roll threads in plastic, steel, aluminum etc. It has been in the tool carousel for a year or so and gets used a few times a week for fixtures and other general purpose work.

[graemeian]

Sorry about the "od" typo. I do not see an edit feature.
Well I thread formed several hundred feet in the 6061 aluminum. ( ~1000 holes). The tap still looks like it just left the package. I did not even mark it as used. 49,000 holes left. Thanks.

[tom o]

I'm new to this ridgid tapping we have tried it a few times using regular collets and was wondering if it was really nessisary to spend $800.00 US on collets that have the tap drive built into them.

[graemeian]

I use taps everyday in my milling center. Mostly 1/2" and under. Form taps up to 3/8". I have only used common collet holders and I have yet, I think, had a tap break due to slippage. As a safety precaution, I always divide spindle speed by feed to make sure it matches the tap pitch. I have had bad luck with helical taps due to material wrap.

[rcs60]

i use regular er collets when rigid tapping for anything 1/2 and under -- over i prefer the tap collet as it drives the tap better with no slippage
tap collets er16 are about $100.00
regular er16-er32 are less than $30.00

[tom o]

Thanks for the replies, that is what I was thinking but it is nice to confirm thanks.

[RCaffin]

I suspect that 2000 RPM might be instant death on the tap, especially on 6061.
To get anywhere near that you would need to drill the holes rather close to the nominal thread OD, but then you would have rather poor thread depth.
You would also need to keep up the supply of cutting/threading oil.

Cheers
Roger

[rcs60]

RCaffin
I suspect that 2000 RPM might be instant death on the tap, especially on 6061.

I think that tapping RPM is dependent tap size, surface feet per minute and on the machine being used
manual machines you go slow to keep control of the process with the addition of a tapping head you could go faster
for cnc machining centers again this is dependent on you machine i had a tree 320 and an old haas vf2 that i wouldn't go faster than 500 rpm
i now run a haas vf2ss,okuma vmc the rpm's most times in the 2000-2500 rpm
as i said in a previous post with the robodrill rigid tapping was done a 4000 rpm and 125 ipm for about 5000 holes with 1 form tap
the haas and okuma i limit to about 2000-2500 rpm is because at some point the machines can not wind up and wind down the bigger spindles along with the bigger servo motors as quick as the robodrill this causes you to program a higher R Plane to let the spindle/z axis get themselves sync'd up to make good threads
you have to experiment with the machine being used to find out where the best tapping speeds are for it
in some other posts people are saying to run the spindle faster so that it lets the timing mark of the spindle be read more often creating a better thread not sure if they are right or not but experimenting with your machine is the only way to get the answers to how fast to thread

[RCaffin]

Thinking a bit more about this - I have to assume you are threading a through-hole, not a blind hole, yes?
I could not stop a 2,000 RPM spindle fast enough for a blind hole!

I was form-tapping M2, M2.5 and M3 in 6061 and 7000-series, in blind holes.

Cheers
Roger

[rcs60]

The machine and process is what dictates the speed of tapping
the robodrill i work on is new and the manufacturer claims tapping at 5000 rpm rigid tapping
the hole was a blind hole .375 deep (9.5mm ) tap was 6-32 (about 3.5mm od of tap ) tapped 3/16 deep full thread(4.7mm )material was steel 12l14

[mactec54]

I suspect that 2000 RPM might be instant death on the tap, especially on 6061.
To get anywhere near that you would need to drill the holes rather close to the nominal thread OD, but then you would have rather poor thread depth.
You would also need to keep up the supply of cutting/threading oil.

Cheers
Roger

2000 RPM could be considered slow for some machines that are designed for high speed tapping, the normal tap / drill hole size is used that you use for a roll form tap you are using, small sizes like this you can run them as fast as the max rigid tapping is for the machine you are using, a roll form thread is stronger than what a regular cut tap can do

Regular coolant that the machine is using is all that is required

[mactec54]

Thinking a bit more about this - I have to assume you are threading a through-hole, not a blind hole, yes?
I could not stop a 2,000 RPM spindle fast enough for a blind hole!

I was form-tapping M2, M2.5 and M3 in 6061 and 7000-series, in blind holes.

Cheers
Roger

Any mill built today can run at these and much higher speeds for tapping, blind or through holes makes no difference, old machines have poor spindle control are what they are slow

[RCaffin]

Um. Not sure I understand all this.
6-32 - that's 32 tpi?
Tapping 3/16" deep: that's 6 threads?
You will probably have to stop the tap in half a turn - from 5,000 RPM?

Does the machine walk across the floor with each reversal of the spindle?

How long does the tap last when subjected to the shock loading of hitting steel at 5,000 RPM?

Cheers
Roger

[RCaffin]

Perhaps the spindle can do 5,000 RPM. But the speed recommendations I have seen from mfrs of thread forming taps seem to vary between 300 RPM and 800 RPM, and even lower above M10.
They also recommend neat heavy cutting oil rather than ordinary coolant. They need some serious lubrication.
They also recommend room at the bottom of a blind hole of at least 2 turns, as the taper on the tap will be around 1.5 turns or more. Actually hitting the bottom is a bit of a no-no.

5,000 RPM would be fine for thread milling with a single point cutter of course, I have done plenty of that. Works well in blind holes too, but you need to air-blast the chips out.

Cheers
Roger

[mactec54]

Perhaps the spindle can do 5,000 RPM. But the speed recommendations I have seen from mfrs of thread forming taps seem to vary between 300 RPM and 800 RPM, and even lower above M10.
They also recommend neat heavy cutting oil rather than ordinary coolant. They need some serious lubrication.
They also recommend room at the bottom of a blind hole of at least 2 turns, as the taper on the tap will be around 1.5 turns or more. Actually hitting the bottom is a bit of a no-no.

5,000 RPM would be fine for thread milling with a single point cutter of course, I have done plenty of that. Works well in blind holes too, but you need to air-blast the chips out.

Cheers
Roger

You could not even compete if you could not do rigid tapping at 1000 RPM to 2000 RPM today note just regular coolant works fine

May be this will give you a reality check they are threading at 8,000 RPM in this video they are doing M6 and M20

https://www.youtube.com/watch?time_c...&v=NsYR8X6fndc

This one shows 3 type of threading

[graemeian]

[I thread formed a lot more small holes. I did drop the rpm to 1600. I did break a tap but it was due to a trash or something in the collet causing excessive run-out. With a new tap, I checked the shank run-out with an indicator and form tapped several more hundred holes.

[graemeian]

I tapped a different thread size and it was the last operation and I used the vactra oil from the manual lathe with a brush wipe on the tap and over the holes. I manually hand tapped form threads for the first time and I noticed the difference oil makes.

[mactec54]

I tapped a different thread size and it was the last operation and I used the vactra oil from the manual lathe with a brush wipe on the tap and over the holes. I manually hand tapped form threads for the first time and I noticed the difference oil makes.

What Vactra oil did you use