What's new
What's new
By:
Advanced search…

Form tapping M12 in 4140PH?

T

trochoidalpath

Cast Iron
Joined
Jan 17, 2016
Before I do something super dumb: I need to tap M12x1.75 through a 40mm thick 4140PH ground plate on a 16K Speedio. Haven't worked much with 4140, and the part has a fair bit of time into it, so I'd appreciate a quick sanity check.

My plan is to spot, drill to 11.2 mm with a carbide CTS drill, and then form tap. OSG ADO drill and XPF form tap in ER25 holders.

Am I going to regret it? Or am I going to run out of spindle torque and just stall out? Should I just plan on thread milling this instead? Thanks in advance!
 
You may live to regret it, but I sure as hell want to see it happen.
Personally, I have never form tapped anything except aluminum.
 
Wouldn't go with it.
Hardness will be close to 30 HRC in 4140PH, almost upper limit to what a general form tap can.

Threadmill. Or SPPT tap.

And you better use tap collet or synchronised tap chuck instead of plain Jane ER25...
 
I have to agree that it could be asking for trouble. I form tap 1/2"-13 in soft 1045 on a small lathe, and it requires a lot of torque- pretty much all my machine has got.

If you do decide to give it a go, do some tests starting with a larger pre-drill than you think you need. That will require significantly less torque than the proper drill size. Watch the tapping torque and see if you feel comfortable going with a smaller pre-drill.
 
I form tap harder materials all the time. 17-4 mainly, up to H900 (low 40's Rc).

I have one part in 36CrNiMo4 QT (4340/EN24) that I form tap M8, made about a thousand of those in the last year or so, never an issue.

Can't think of anything explicitly 4140HT that I form tap, but I can't see it being an issue from the tap's perspective.

Whether or not your machine can manage it, I don't know. I form tap up to M16 regularly, but I have bigger machines.
 
Thanks for your feedback everyone.

I’ll try to find a thread mill with enough reach — that might be tricky. If I can’t find a reasonable one, I’ll probably try it with a spiral point cut tap.
 
Why not test it on another test article first? 10K spindle will tap M16 holes to structural steel, but probably not in 4140. You might possibly have to run it at higher RPM than suggested by calculators to obtain more torque from the motor. I have slapped regular tapping paste for M16 just to make sure the lubricity is there. Maybe you could drive small start with the machine and hand tap to finish, just something my cheap ass would do before investing in new tools..:)
 
Would peck tapping not be a viable option ?. I only ask because I haven't tried it yet on my 10k S500. 1/2-13 in 1018 through 1/2" plate is as much as I've needed so far.
 
Carmex Part Number MT 0808 C28 1.75 ISO has a usable length of 28.9mm... So if you're comfortable relieving the shank by another 11mm on your own, that'd work, and probably be cheaper. They make some thread mills with the LOC you need, but only in 1.5 or 2mm pitch, not sure how the 1.75 got skipped.

That's the best I could find for you right now, I'll have a look at some other catalogs later.
 
I feel that as a general consensus we could all agree that when in doubt thread mill if your having second thoughts. These type of posts pop up quite often sometime size related or difficult material issues. Sure threadmilling takes more time but is very predictable once you’ve dialed in your settings. Look at the tourqe values it takes to drive a large tap vs the tourqe curve of your spindle, the machine may be able to do it, but do you really want to subject your precision spindle to those forces?
 
What forces? Tapping has no force other than torque, surely you've experienced this by hand. Roughing or facing is much tougher on a spindle.

Finding a decent tapping torque calculator was online was tough. Walter has what seems like a good one. Walter Machining Calculator It looked like in P8 it's 33Nm for M12 and the Speedio has 40Nm? OSG The OSG catalog estimates the same in 35HRc.

I'm just an amateur, but when I had a tiny machine I figured out I had to calculate Tq and HP for all bigger cuts and drills, never stalled the spindle again.
 
gregormarwick said:
I form tap harder materials all the time. 17-4 mainly, up to H900 (low 40's Rc).

I have one part in 36CrNiMo4 QT (4340/EN24) that I form tap M8, made about a thousand of those in the last year or so, never an issue.

Can't think of anything explicitly 4140HT that I form tap, but I can't see it being an issue from the tap's perspective.

Whether or not your machine can manage it, I don't know. I form tap up to M16 regularly, but I have bigger machines.
Click to expand...


A Brother can doo anything that your bigger machines can, and faster!
(sounds like an Arctic Cat rider talking)


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

Think Snow Eh!
Ox
 
dieselpilot said:
Finding a decent tapping torque calculator was online was tough. Walter has what seems like a good one. Walter Machining Calculator It looked like in P8 it's 33Nm for M12 and the Speedio has 40Nm? OSG The OSG catalog estimates the same in 35HRc.
Click to expand...

16,000 RPM spindle is only good for 27 Nm instantaneous (my 2016 S700X1 anyway), so maybe it makes it, maybe it doesn't.

Regards.

Mike
 
Finegrain said:
16,000 RPM spindle is only good for 27 Nm instantaneous (my 2016 S700X1 anyway), so maybe it makes it, maybe it doesn't.

Regards.

Mike
Click to expand...


rocky-drago-if-he-dies.gif
 
You didn't say how many holes or how many parts. I assume just one plate?

If just one plate I would absolutely not form tap it. I had a job recently, 300 little 303 stainless bullet nose things (lathe work) with a 10-32 hole. I read a bunch of these posts and figured sure form tapping works fine on 303. Bought the tap, first part, tap broke. Switched do a spiral point tap and did the whole bunch no problems. Probably if this was a job that was worth a the process development time and money it would be worth it but for one part I would go with thread milling. Or if just a few holes I think I would just tap them with a cut tap in a little and finish them by hand. But I think a single cutter thread mill ought to work.
 
Pete - you did drill the hole bigger than normal eh?

You shouldn't have had that experience under normal conditions.

???


This isn't exactly the right thread to post this, but since we are kind'a there anyway....

I had some 304 parts to tap the other day, and I have never found 304 to tap in a coolant machine with a cut tap and not break it.
I found a used OSG form tap and went to work. (only had 18 holes)
The tap broke straight away, and I didn't think that I had anymore taps like that in stock, but in a different app drawer I found a box of form taps this size from Jarvis.
I used to buy many form taps from them 20 yrs ago, but I don't feel that forms are the best option most times, so I have gravitated more towards Mod Bottom SP FL taps from OSG or Morse, or similar.

But anyway - there was a whole box of the right sized taps from Jarvis here, so I tossed one in, with hesitation....

I got WAY better results with that (also used) TiN coated Jarvis tap than I would have gotten with a brand new TiALN (?) coated OSG! :eek:

I had noticed on other similar jobs where I am tapping 304 (these are normally just short runs of weld-on lugs) that even a brand new (OSG) tap produces a very warm part, and even steam will come out of the spindle bore when I re-chuck parts. The Jarvis parts all came off cool.

These results with proper hole size, not overboring like y'all like to doo.


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

Think Snow Eh!
Ox
 
You must log in or register to reply here.

Similar threads

M
Uncoated form tap in steel? Will this work?
Replies
10
Views
1K
Mtndew
Mtndew
T
Standardizing Form Tap Tip Geometry
Replies
13
Views
973
Trevor360
T
M
Metric STI Threads - Roll Forming
Replies
9
Views
1K
LKN thread insert
L
M
Adjustable torque tap holder clutch life
Replies
1
Views
382
Strostkovy
S
R
Advice on Tapping 3/8-24 hole in 316
2
Replies
24
Views
2K
Blaser Swisslube
Blaser Swisslube








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top