I need to tap a bunch of blind holes in 6061, 2 mm x 0.4 x about 10 deep. I've not done small stuff like this before. Should I use a floating holder or rigid tap? What speed would be a conservative starting point? Hoping not to break too many of these dinky taps. I usually tap very slowly (usually in SS), but there are about 800 holes to do here.
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Small taps in aluminum?
- Thread starter swarf_rat
- Start date
- Replies 21
- Views 4,781
stroker
Hot Rolled
- Joined
- Jun 23, 2006
- Location
- Melbourne Australia
I'd be inclined to form the threads on a machine with rigid tapping.
I've had success forming M4 x 0.7 20mm deep in 304 stainless with these:
https://www.walter-tools.com/SiteCo...en-gb/handbook-drilling-threading-2009-en.pdf
Good luck.
I've had success forming M4 x 0.7 20mm deep in 304 stainless with these:
https://www.walter-tools.com/SiteCo...en-gb/handbook-drilling-threading-2009-en.pdf
Good luck.
G
Guest
Guest
Whatever you do a good quality aluminum will save a lot of nightmares, say no to Chinese crap.
JP Machining
Stainless
- Joined
- Jul 15, 2006
- Location
- Wisconsin
Done alot of M2x.4mm in 6061 Kaiser select precision rod. Form tap, held rigid in collet chuck. Push my old Haas to 2500 rpm tap speed and go. If it would handle rigid faster I would but I think its only rated for 2k. One tap is on aprox hole #9k
What machine?
I would tap as fast as your machine can tap accurately. Rigid tap.
Of course on our Brother I would go 6k rpm, but on our Hyundai-Kia Fanuc 0 mill, I wouldn't even try it because the spindle can't stop and reverse fast enough, so about 300rpm max.
Our Okuma mills I would go about 3k rpm or so.
I am unfortunately familiar with foreign aluminum and always buy US sourced product. The machine is a DMC63V, not sure what speed it might be rated for. The positioning is accurate (glass scales) but how quickly it can start or stop I don't know.
G00 Proto
Hot Rolled
- Joined
- Feb 18, 2013
- Location
- Dirkdirkistan, ID
I don't get to carried away with tap RPM... 500 for prototype and 1000 for production. Prevents math errors and I think it is easier on the machine. On 800 holes I wouldn't get to excited about the potential improvement in cycle time to go up into the multiple of thousands.
I have had difficulty with small threaded holes in aluminum. The threads looked fine and I didn't break many taps, but I have had issues getting them to pass QC. Whenever I get much below 2-56, I have a tendency to ream the holes after drilling. I consider the error in hole diameter and the subsequent impact to the other thread dimensions to be a percentage, rather than a straight numerical error. In other words, a couple thou error in diameter on a 1/4-20 is much less significant that the same diametrical (big word bonus points) error in a 0-80... unfortunately, my potential error in drill diameter seems to be about the same regardless of drill size.
I think that some of the modern stub length carbide "engineered" drills can hold drastically better tolerance than the old HSS jobber drills, but it seems to take more fiddle fucking with drill sizes and cutting conditions than ordering reamers in a couple tenth increments and picking the one that gages out correctly. Especially considering the relatively low volume of holes you need to tap.
I have had difficulty with small threaded holes in aluminum. The threads looked fine and I didn't break many taps, but I have had issues getting them to pass QC. Whenever I get much below 2-56, I have a tendency to ream the holes after drilling. I consider the error in hole diameter and the subsequent impact to the other thread dimensions to be a percentage, rather than a straight numerical error. In other words, a couple thou error in diameter on a 1/4-20 is much less significant that the same diametrical (big word bonus points) error in a 0-80... unfortunately, my potential error in drill diameter seems to be about the same regardless of drill size.
I think that some of the modern stub length carbide "engineered" drills can hold drastically better tolerance than the old HSS jobber drills, but it seems to take more fiddle fucking with drill sizes and cutting conditions than ordering reamers in a couple tenth increments and picking the one that gages out correctly. Especially considering the relatively low volume of holes you need to tap.
Pete Deal
Titanium
- Joined
- Apr 10, 2007
- Location
- Morgantown, WV
I never have done M2 but lots of M3 holes. I will second what G00 Proto said- start by making sure your hole diameters are what you think they should be before you start tapping. I gone wrong here before.
I think I'll try a rigid holder and start at 500 rpm to see how it goes. The hole diameter thing is why I'm reluctant to use form taps for this or other short runs. There are numerous studies indicating that formed thread are great - provided you have exactly the right pilot hole diameter. Otherwise, they can be crap and still pass QC because of the formed shape. In long runs you can spend the time to get them just right. Cut threads on the other hand can have fairly large variations on pilot hole without big changes in strength.
Rick Finsta
Stainless
- Joined
- Sep 27, 2017
On a Speedio I would run that rigid with a form tap at 6k RPM.
Finegrain
Diamond
- Joined
- Sep 6, 2007
- Location
- Seattle, Washington
Oh geez, don’t get us Speedio guys going, we’ll never shut up 
The spindle accel/ decel is PDQ. I would not be surprised if my S700 could hit 6,000 in this scenario, but I don’t really know.
Regards.
Mike
The spindle accel/ decel is PDQ. I would not be surprised if my S700 could hit 6,000 in this scenario, but I don’t really know.
Regards.
Mike
BROTHERFRANK
Stainless
- Joined
- Dec 20, 2013
- Location
- SoCal
Speedio spindle takes less than .1 seconds to get to 6k. At 6k it's almost like a light switch. You can go from M3 to M4 at 6k and you might not see it reverse. Here is a video of Synchronized tapping on Brother:
YouTube
Last edited:
Nerdlinger
Stainless
- Joined
- Aug 10, 2013
- Location
- Chicago, IL
I am curious - is there some accuracy “standard” a tapping process must conform to in order for it to be considered “rigid tapping”? I am knee-deep in a rigid vs non-rigid tapping situation at work so it’s on my mind. I am thinking something like, “spindle rotation must be within “x” degrees of theoretical position for a given linear position as a function of thread pitch.” or something. On that note, how “off” is a machine without rigid tapping? Like - what’s the difference in terms of real numbers?
gustafson
Diamond
- Joined
- Sep 4, 2002
- Location
- People's Republic
Form tap!
the difference in speed on that machine between 1k and 2k rpm is small. 500 is just silly slow
drill with a standard hole drill, measure actual hole size, tap, check with gauge and also check minor diameter
thread can pass the gage but fail the minor. Even if you have get an odd size drill, it is worth it. The smaller and finer the fussier they are going to get.
you should break zero taps and have that tap for years
I think we get over 20k holes out of #6, maybe 50k I dunno
the difference in speed on that machine between 1k and 2k rpm is small. 500 is just silly slow
drill with a standard hole drill, measure actual hole size, tap, check with gauge and also check minor diameter
thread can pass the gage but fail the minor. Even if you have get an odd size drill, it is worth it. The smaller and finer the fussier they are going to get.
you should break zero taps and have that tap for years
I think we get over 20k holes out of #6, maybe 50k I dunno
hanermo
Titanium
- Joined
- Sep 28, 2009
- Location
- barcelona, spain
I am very interested in the final result.
Please post.
Have no doubt the brother spindle, as a servo motor, can get to 6000 rpm in 0.1 secs, as posted previously.
At 6000 rpm, 0.4 mm / rev, or 100 revs/sec, it would be ..
.. 25 revs (10 mm deep) in 0.25 secs.
If the brother spindle can reverse in 0.1 secs, this would be 10 revs or 4 mm in depth at 0.4 mm/rev from 6000 rpm.
Very curious to know actual specs and actual results.
Please post.
Have no doubt the brother spindle, as a servo motor, can get to 6000 rpm in 0.1 secs, as posted previously.
At 6000 rpm, 0.4 mm / rev, or 100 revs/sec, it would be ..
.. 25 revs (10 mm deep) in 0.25 secs.
If the brother spindle can reverse in 0.1 secs, this would be 10 revs or 4 mm in depth at 0.4 mm/rev from 6000 rpm.
Very curious to know actual specs and actual results.
I’ve had good luck with them.
Well, I started at 500 rpm and had no problems. Upped it to 1000 and still no problems. Upping it above that yields little in cycle time improvement (since they are shallow holes).
I've got a couple of Tapmatics, the problem in a CNC machine is the reaction bar. Spindle and tool changer have to be able to deal with it, depending on circumstance this may be difficult or impossible. In a Bridgeport or drill press sure, they are great.
I've got a couple of Tapmatics, the problem in a CNC machine is the reaction bar. Spindle and tool changer have to be able to deal with it, depending on circumstance this may be difficult or impossible. In a Bridgeport or drill press sure, they are great.
