4-40 helicoil taps

[Justin Beebe at Folsom Tool]

I have a job coming up that requires six 4-40 helcoil tapped holes per part. The material is 303 stainless. The tapped holes are though holes and the material is .180 thick. We will eventually be making thousands of these parts. I don't normally tap holes this small. I am thinking of using Emuge spiral point taps. Can anyone offer any advice as to tap brand or possible feeds and speeds. Also the info I looked up on the drill size for a 4-40 helicoil says to use a #31 drill. Does this sound correct?

 

Thanks

[Justin Beebe at Folsom Tool]

I also forgot to ask. I have the option to rigid tap or use a floating tap head. What do you guys recommend.

[Hardmill]

Justin in the unspecified uploads folder on the ftp

theres a file named "Main HC-2000.pdf" that

has all the helicoil data in it.

 

And rigid tapping is the way to go.

 

 

PEACE

[Dave.L]

If you can, form tap these. Look at Guhring taps, they are awesome and about 1/2 the price of Emuge and as good or better performance.

[TK-32™]

303 is not hard

[Dan@home]

303 SS taps nice as TK-421 says. Most any tap.

[35K chipper]

get a helicoil gun if you get all those parts and a few tang breakers and the proper length helicoils.

hole prep. is very important its all in the helicoil book.

 

35k

[Justin Beebe at Folsom Tool]

Thanks you guys for all the replies. I am going to get the helicoil PDF Hardmill. I will also look into the Ghuring taps since I will be using Ghuring drills on these parts. 35K Chipper we are still trying to get permission from the customer to install the helicoils. We may just drill, chamfer, and tap them.

 

Thanks again

[35K chipper]

make sure it's the right angle on the cham. 120deg.

i think check the book!

 

35k

[gcode]

When threading small holes I always drill or even ream the hole to the high end of the hole size tolerance. Even a couple of thou'

can make a big difference when tapping small holes

[Justin Beebe at Folsom Tool]

It is 120deg. on the chamfer and it also gives the chamfer size.

 

Thanks again

[Justin Beebe at Folsom Tool]

gcode, thanks for the good advice.

[Dave.L]

If you use good solid carbide drills, 135 or 140 point, self centering, you won't need to ream the hole since the drill will be within .001 all day long.

[Philcott]

A question for the engineer who designed this part.

 

Why would you need to use a helicoil in 303 stainless? Aren't helicoils usually made out of stainless and if so doesn't is seem like a lot of work to put a Stainless helicoil in a stainless part. I don't understand the advantage.

 

quote:

---

Even a couple of thou'

can make a big difference when tapping small holes

---

You ain't just whistling Dixie there Gcode

[35K chipper]

good question unless they are using the self locking helicoils for some reason.

 

35k

[gcode]

A couple of weeks ago I finished a project that

involved drilling and tapping a thousand plus

blind 10-32 holes in a 304 SS weldment.

We did it without breaking a single tap.

I learned a few things in the proccess I thought I'd pass along.

I used OSG EX-GOLD stub drills so no spot drill was required and drilled them to the max size

allowed in the thread charts

These drills worked well but were too slow

Next time I'll try solid carbide drills

 

The tap was an OSG coated roll tap.

They come with 2 different tapers on the tip..

The mild taper worked MUCH better than the bottom taper.

 

What surprised me was how much the chamfer affected tap life and performance.

 

120 degree chamfers gave a lot of problems, poor tap life and trouble starting threads with floating holders. A couple of holes had the first couple of threads chewed up becaause the floating holder didn't bite.

 

90 degree was better.. 60 degree was the best

Tap life in 60 degree chamfered holes was triple that of a 120 degree hole.

 

It makes sense when you think about it.. but I thought I'd pass it along.

[Dave.L]

quote:

---

304 SS weldment

---

Was it stress relieved after weld?

 

This reminds me of a nightmare about 6 years ago. Welded parts, 6-32 tapped holes. It cost us more in EDMing the broken taps out then the job was worth. We determined there must have been hard spots in the material because in some places it tapped just fine.

[gcode]

quote:

---

Was it stress relieved after weld?

---

no.. it was tough sledding too.. along with

all the tapped holes there was about 1000 inches

of dovetail groove.. some of it right next to 8"

high walls.. I wish I could put up pictures but..

[Dave.L]

Big dollar part I'm sure.....I hope...

[Justin Beebe at Folsom Tool]

PhilCott

 

I asked that same question today to a guy I work with who used to work for the company we are making these parts for. He looked at the engineers name on the drawing and told me the engineer died a long time ago. So I guess we will never know the answer to that question.

 

So what I am going with is:

 

1. Drill with 3.1mm (.122) diameter Guhring series 5514 solid carbide drill 140 degree with FireX coating (minor is .117/.125)

 

2. Chamfer holes to .155 diameter with 120 degree 6 flute chatterless solid carbide countersink (gcode if it gives me any problems and I can change the angle I will)

 

3. Rigid tap with OSG 4-40 STI spiral point taps. I can't remember the exact tap exo- something. I couldn't get the Guhuring or Emuge but I heard these OSG's are excellent

 

These part went out to double disk grind today so I will be finishing them in a few days. I'll let you guys know how it turns out.

 

Thanks for all the advice

[mcpgmr]

I can tell you how to get a perfect hole every time but since you don't return my calls I'm holding out! J/K

[Justin Beebe at Folsom Tool]

Paul,

 

I did get you message and have been meaning to call you. I'll give you a buzz tommorrow. I'd like to hear about your job. I have only made one program for our Deckel but I may still be able to get some answers for you.

 

 

I apologize for the delay

 

Justin