Tap

[Don Clement]

I am using the Balax equivalent of an H5 tap meaning that the tap is 2.5 mils oversize. That is about 1 drill size larger. Also it depends on the material one is going to form tap. That's why I said to try a form tap first and then adapt from the Balax recommendation (starting point really )for the particular material, the tap oversize or H limit (or in Balax case B limit), and the tapping fluid used for one’s specific application. It’s about adapting to one’s particular application or survival of the fittest in the evolving world of CNC.




“If you always do what you’ve always done, you’ll always get what you’ve always got.”

[Don Clement]

roll taps are the way to go , especially with deep holes and smaller diameters .
i've run numerous tests on roll tap vs cutting tap , tests were based on three threads and how much torque it took to strip , then 4 threads and so on till bolt heads snapped before stripping the thread . both were pretty much equally the same in stripping strength in 6061 .

My experience with tens of thousands of form tapped 4-40 holes in 6061-T6 is excellent. I used a minimum depth of 8 threads with a SS black oxide coated Allen socket button head fastener. Initially there were intermittent results sometimes the heads would break or the threads would strip. Eventually I got the process down to heads would never break and threads would never strip. I believe there were many factors that determined good results such as how much torque was applied and how fast the torque was applied or if torque was applied in two stages with a rest period in between. So I can’t say with certainty what factors contributed to the final result except that forming taps work extremely well for me in my application. YMMV

Don

[dertsap]

My experience with tens of thousands of form tapped 4-40 holes in 6061-T6 is excellent.

Don

Like you I've had great success with roll taps on the hundreds of thousands of 4-40 holes that I've tapped over my career .
my point was that roll form threads in 6061 is not stronger than cut threads .
I needed to test to see which thread was stronger , I currently work with medical products and we cannot afford for threads to fail . We can't have customers over tighten the equipment , strip the threads then blame us for faulty products , we need bolts to snap before our parts fail (which would be to an extreme) .
When I requested to introduce form taps to the machining process I was told to test the thread strengths between roll and cut taps , the point was to strip threads and to snap high grade bolts and to document the results .
The documentation consisted of how much torque was required to strip each of the threads which had an equal thread percentage at each given depth .
I tried threads at a variety of thread percentages and each at different depths . The results for both forms of tapping required nearly exactly the same amount of torque to strip the threads out , and both were equally the same when it came to the point of busting the heads off of the cap screws .
these tests were done numerous times and the averages were documented . This proved that roll taps would be sufficient for the products we manufacture but it has also proven to me that in the aluminum both threads are equal in strength .
Other materials may and probably will differ but that's not my concern at this point of time
.

[Don Clement]

This proved that roll taps would be sufficient for the products we manufacture but it has also proven to me that in the aluminum both threads are equal in strength .

As you say, your results have been ostensibly proven to you. Were your results published and reviewed? Were others able to reproduce the tests and get the same results?

Don

[dertsap]

As you say, your results have been ostensibly proven to you. Were your results published and reviewed? Were others able to reproduce the tests and get the same results?

Don

No , i work in a machine shop and not a lab so tests were done and the notes were turfed !
I suggest that if someone feels the need to know the facts then they run their own tests rather than believe that the threads are stronger because someone else says so

[rowbare]

You got me googling...

It would seem to make sense that threads with the same characteristics would have similar strength. In the both cases you end up with the same thickness of material at a given point along the thread pitch. The tapping action doesn't change the metallurgy so the strength of a .010" cross section isn't going to change significantly (though according to this article there is an increase in tensile strength due to changes in grain pattern: Rolling Threads Has Advantages : Modern Machine Shop). Most field testing methods would not be sensitive enough to measure this difference. In the end 6061 is 6061 no matter how you machine it.

There is a work-hardening effect when forming threads so you will end up with a tougher thread. This may be important in a case where fasteners will be frequently removed. According to this article, rolled threads are much more sensitive to hole size than cut threads: Internal Thread Strip-Out Tests Yield Surprising Results | Machine Design

There is a good discussion here: Is there any sort of factor that relates the strength of rolled vs. cut threads? [Archive] - The Home Shop Machinist & Machinist's Workshop Magazine's BBS

Oh another interesting article on the subject: http://www.ctemag.com/dynamic.articles.php?id=197

I like threads like this. Makes me learn things.

bob

[tbaker2500]

So I bought my first forming tap, for 4-40, to try it out after following this thread. I have a new favorite thing! Man it's that much easier on a blind tap, not having the chips. Thanks for the info!

[beanbag]

I recently tapped a buttload of blind holes with a roll tap in aluminum. I think it was some guy named Ox either here or on Practical Machinist that said to use a high thread percentage for small threads, and I agree with that. Balax called for a .109 drill as default, and I ended up going all the way down to .1065 until I stopped getting that annoying double crest feature that makes cross-threading more likely. (I did that technique where you first drill undersize and then re-drill with the final size to get the most consistent hole size possible.) That Ox guy also said something about internal rolled threads not really being stronger because of this double crest.

[tbaker2500]

Pretty! Thanks for the info.