thread forming 316 stainless steel and adequate percent thread engagement

[cgrim3]

Hi all,

At our shop, the majority of the work we do is on 316 stainless steel, inconel, and titanium 6Al4v. Out of those, we do 316 stainless the most. We mostly use emuge cut taps and carmex thread mills to create female threads. I would like to get into thread forming with form taps since there are no chips produced and it's easier to tap a blind hole, plus the threads are stronger. I bought some emuge innoform roll taps specifically for 316 Stainless in 1/4-28 and 5/16-18 sizes to test out in a scrap block of 316 stainless to see if it would pay off to use these taps for a production job.

When we use cut taps, I just follow the tap drill recommendation on the drill chart on the wall in our shop. If I remember correctly, I think your standard tap drill size from a chart allows for 75% thread engagement. I read that online somewhere but can't remember where.

I read that the strength difference between 75% thread engagement and 100% is only 5% but it takes 3 times more torque to tap a hole with 100% thread engagement than 75% thread engagement.

I know hole size is critical for roll taps, so my question is what percent thread engagement should I shoot for when tapping 316 Stainless in general? is 75% engagement too high? FYI Our customer typically does not call out thread class on their drawings. Regardless I have to know the percent thread engagement so I know what size to drill the hole for the form taps. I just need guidance for this since it will be my first time using roll taps. Also, should I peck tap the roll taps when rigid tapping or not? Should I ream the hole with a reamer to get it close to the size I need (or could just ream with a drill when close to the size) or should I interpolate the hole with an endmill?

FYI we are using emuge tapping fluid for tapping.


Thanks,

Chris

 

[Scruffy887]

Hole size is important and not so sure about 75%. I have been roll tapping 304 for over a decade, but that is a repeat job. Forget what drill I used for 1/4-20. But for sure you need to pay attention to tool life. The edges will start to fail/gall and not so easy to see with naked eye. May not break at that point, but may not allow a screw to be threaded into the hole either.

 

[DanASM]

I got into roll threading last year on a 316 job. 5-40 TiCN form taps from OSG or Ghuring. Go for the expensive ones, they are worth it.

I am getting 3000-5000 holes at .300" deep. #32 Drill.

When my taps break it is due to me dropping the toolholder or some other human error. I havent gone smaller than that yet or bigger for that matter.

Screw Machines with oil. lots of oil. Taps love it. No Chips is great. Threads get cold worked and are pretty hard at 60-65% Threads.

 

[Goff]

To the OP. Most tap suppliers have the information to calculate tap drill sizes in their catalogs.
I copied this:

Inch tap drill= Nominal thread OD — (.0068 x % of Thread Desired) ÷ TPI

EXAMPLE: 1/4-20 Tap with 65% Thread) = .250 — (.0068 x 65)/20 = .228” Dia.


Metric tap drill= Nominal thread O.D.(mm) — (% of Thread Desired x mm Pitch) ÷ 147.06

EXAMPLE: M8 x 1.25 Tap with 65% Thread) = 8 — (65 x 1.25) ÷ 147.06 = 7.45 mm Dia.

 

[tntcustom]

I started my form tapping adventure on a 316 SS job as well. 1/4 20 and 10-24. I later ran a ton of trials on a job in A572-gr50 plate, FORMING M30x3.5 thru 2” plate(yes you read that correctly), using Jarvis, Guhring, Widia, (all custom made) and the eventual winner OSG A-Oil taps(from Japan not the USA A-tap that’s a cut tap).
Definitely worth it. I thread form daily in a job shop. After you figure it out it’s no harder than cut tapping.
OSGs website has a killer chart for threadforming drill sizes under tech. You don’t need to know % or calculate anything. Just look at chart and go at it.

I 100% recommend solid carbide drills or replaceable head type for larger sizes. Ex, 1/4-20 is a .2244 solid, M30 is a 28.4 or 28.3 mm Sumitomo SMDH style drill depends on class of fit.
IMO 3000 holes is low for small sizes. We achieved 4-6k holes in m30 with semisynthetic water soluble coolant from trim, at 8% concentration, but we did add 5% of their chlorinated lubrication additive.

I agree most I break are from either drills going dull or pushing up in the collets, or from being dropped.

1 caution , in vertical machine without CTS, we add a stop to have operators blow out the holes right before tapping. The tap makes no chips to jam, but if you drill a hole pattern chips from one hole can fill up the previous holes and cause issues.

 

[Orange Vise]

316 work hardens readily and things can go downhill fast with form taps, but the benefits are obvious if you get it right.

I wouldn't experiment on a high dollar part.

I'd also recommend rolling out the new tooling slowly, i.e. don't change all your programs at once just because the first tests went well. BTDT, not fun.

The tap manufacturer should provide drill size recommendations.

 

[Conrad Hoffman]

One caution with rolled threads. They will have a slight crease at the top of the thread and if assembly is done by the unskilled or the uncaring, it's easier to cross thread the fasteners because they catch on the crease. Be sure your customer is OK with formed threads. Me? That's all I'd ever use.