CNC machining m1 threads into 304 stainless

[justin8888]

Hi all,

Im designing a small part where size constraints force me to use m1 x 0.25 screws. The material is 304 stainless (18-8). Ive had 2 shops tell me they cant do it and one shop tell me they can, though the guy who told me they can was more of a product manager type and i dont have an official quote from them yet.

This has me concerned that the design may not truly feasible. I just wanted to get some general opinions on if this is a reasonable operation to request as I continue to source suppliers.

thanks

 

[Bill in PA]

You have not provided much information to get reasonable responses. If the issue is that no one wants to tap 1mm holes in 304, what about using 303? Or perhaps installing thread inserts that are made of an easier to tap material?

More details about your part will help. Posting a drawing would be best.

Bill

 

[Conrad Hoffman]

Finding decent M1 taps is an exercise in itself, but I think with careful selection of the tap drill, and the right lubricant, you can form tap it. I know there are cutters so you can mill it, but why would anybody want to?

 

[litlerob1]

Guhring, Balax and OSG all make M1-.25 Taps. Without question others do too, those are just some names I like. Point is, if someone is making the Taps--someone is using them! It is a tiny tap, but there are smaller.

Find a shop that does Medical, Aero, Mold work, Electronics that is normal for them, Joe Shmo and his Bridgeport is not really equipped for it. Not saying it can't be done guys!!! Just that there are shops that do it in their sleep. 0000-160 is a small Tap, but it gets done.

@Conrad, the smallest Threadmill I have seen is for 2-56, but if there are smaller, show us a link or something please. I'd like to see the geometry.

R

 

[dksoba]

We could do that. Send me a PM.

 

[Comatose]

Is the callout for 304 or is it for 18-8? If it is 18-8, then by all means use 303, and that won't be any real trouble to tap. 304 is just so variable that I'd be loathe to try to tap it unless I was using a special grade.

I've also tapped about that small (#00) into 316 without issue. Form tap is your friend, spend extra time making sure your drilled holes are bang on.

1.MMx.25 BH2 MINIATURE THREDFLOER | Balax | Forming Taps, Cutting Taps, Thread Gages

 

[precisionmetal]

I'd think thread milling would be a better option.

PM

 

[Lastu]

Shouldn't be unreasonable. We have done some M1 threads in 316. Not the nicest project in the world but we got through them without too big of a hassle.
(First bought some form taps, but then the job got rushed and didn't want to take any chances so order some threadmills and didn't even break any)

 

[NAST555]

I'd think thread milling would be a better option.

PM

What size is that thread mill?

Ok ok I had to google it. You actually get M1 thread mills! I see OSG stock them. I suppose it would be the way to go or even an M1 tap on a decent machine should work but I have never gone that small. How do you fasten the screw that goes in there without stripping the thread? You guys have sturdier hands and way better eyesight than me!

 

[Conrad Hoffman]

Well, these should keep you entertained-
98M5-125L2FA1 Standard Length Micro Thread Mill M.5 X .125 Series – Kyocera Precision Tools

 

[litlerob1]

Well, these should keep you entertained-
98M�5-�125L2FA1 Standard Length Micro Thread Mill M�.5 X �.125 Series – Kyocera Precision Tools

Woot that is small, glad I know it's out there, thanks.

 

[precisionmetal]

As a small aside... at my last job, we were running a test to check the life of an M1 thread mill in extruded 7000-series aluminum. This was done in a Robodrill at 24,000rpm. We were able to fit a few thousand holes into our test plates. Drill all the blind holes (about 3.5mm deep as I recall), and then thread mill.

Bottom line is, we ran many plates with a single thread mill and finally gave up because we had cut over 15,000 or 20,000 threads with a single cutter, and the very last thread done still passed the thread gage perfectly.

Admittedly... this was aluminum, so this does not reflect on what the OP is doing. However... I remember thinking when we started the test that we would either break a thread mill in short order, or start having threads that wouldn't pass spec fairly soon. Neither happened before we finally gave up.

fwiw.

PM

 

[Ox]

Is the callout for 304 or is it for 18-8? If it is 18-8, then by all means use 303, and that won't be any real trouble to tap. 304 is just so variable that I'd be loathe to try to tap it unless I was using a special grade.

I've also tapped about that small (#00) into 316 without issue. Form tap is your friend, spend extra time making sure your drilled holes are bang on.

1.MMx.25 BH2 MINIATURE THREDFLOER | Balax | Forming Taps, Cutting Taps, Thread Gages

Yep - that was my first thought.
Is your "18-8" spec open for 303? (They're both 18-8)


--------------------------

Think Snow Eh!
Ox

 

[ToolHIT]

In 304 Stainless Steel a Tap that small just won't hold up and Thread Milling is definitely the way to go as long as you aren't going real deep. A M1x0.25 Thread Mill would give you a Max Depth of 0.100". Any Mini Thread Mill would work, I've had the best luck with Carmex's:
Carmex- MTS7C225ISO -Shop ToolHIT

Here are speeds/feeds:
SFM: 225
CLPT: 0.0009"

-Mike

 

[Bill in PA]

Plenty of replies. Where is the OP?

Bill

 

[justin8888]

Plenty of replies. Where is the OP?

Bill

Im here. Appreciate all the comments. I ended up redesigning for for m1.6. Hoping it works out