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

alternatives to tapping inconel 718?

S

shyam

Plastic
Joined
Feb 23, 2021
I have been breaking a awful lot of 1/4-20 taps trying to hand tap Inconel 718. I was wondering if there are any threaded inserts that can be shrink fit or something along those lines to bypass tapping? I dont want to use helicoil inserts as I still need to tap the hole. Any insights or ideas will be appreciated.

The taps are breaking because these are 3D printed specimens that are heat treated to give them thor strength :cryin:
 
shyam said:
I have been breaking a awful lot of 1/4-20 taps trying to hand tap Inconel 718. I was wondering if there are any threaded inserts that can be shrink fit or something along those lines to bypass tapping? I dont want to use helicoil inserts as I still need to tap the hole. Any insights or ideas will be appreciated.

The taps are breaking because these are 3D printed specimens that are heat treated to give them thor strength :cryin:
Click to expand...

So weld or rivet them. No more bustid taps!

:D

Yes. TONS of inserts exist in immense variety for all manner of host material.

Start with Penn Engineering even if only for ideas:

PEM(R) Fasteners – PennEngineering

They have competition. Lots of it. You can easily make your own to suit your particular needs, too. PEM was born off the back of just such a need.

Otherwise? The "host" material is plenty strong enough to HOLD. Folks DO tap it. Often. Seems more than just an avoidable "nuisance" to have to thread-mill?

How hard can it be to arrange to drill and tap BEFORE the heat-treat that is busting yer chops? Er.. 'taps'.

??
 
Unless there is a way to 3D print the threads, even partially, and finish off with the tap, I would seriously look into thread milling with carbide. I've done about 18 tons of Incoloy fabrication over the last decade.

Question: how about having inserts made out of something like 4140 and then TIG them into the hole?
 
Emuge DF NI taps are specifically ground cobalt plus tramps for the dreaded inco nightmare, plus if enough room a jet of coolant down the hole if blind or back coolant up the hole if through, sticky pad and top hat hose end round the back, blow it up, old fashioned forward backward tapping plus withdrawing and flushing, slow but it works
Mark
 
Wow what a pain. Lots of experienced people here who are familiar with this material extensively. Usually it is a confidence and competence thing because material is so very expensive and hard to work. After mastering it it is very good because in General most shops are repulsed by the prospect of jobs with such materials.

The learning curve can be very expensive too much for most shops they just quit before they get bogged down.

Emuge Taps overall have been a bright spot as far as tapping holes is concerned. They are a top notch mainstay for me. Too the thread milling has been fantastic on so many occasions that it hurts to think of the time before I started using the process.

Keep in touch as with the suggestions given I am interested in what you end up doing.
 
If it is 3d printed it really should have the threads at least roughed in as made. Are you reaming the holes before tapping? Can you use a nut and bolt instead.
 
So I cannot weld or rivet them because it has to be removeable. it is a test specimen so it has to be assembled and disassembled. The test is conducted on inconel specimens as it is rotated and a load is applied to it. There are minimal forces on the screw so I think if I am able to find a threaded insert I will go with it.

Furthermore, I am a noob machininst so I think it is also a contributing to the broken taps.


The bar stock is brought heat treated because it is expensive (we found) to send it out to heat treat afterwards from a 3d printing vendor - the vendor prints the specimen, heat treats it and sends it over to us. We are a research lab and we have a few CNC machines in house but we do not have an oven for heat treat/qunching.

THank you so much for your insights.
 
Get the proper grade Taps, in Taper , Plug and Bottom.
Make damn sure your started straight.
As soon as it becomes hard to push the Tap switch to the next, repeat.
Lots of lube.
Lots of patience.
It can be done.
 
shyam said:
So I cannot weld or rivet them because it has to be removeable. it is a test specimen so it has to be assembled and disassembled. The test is conducted on inconel specimens as it is rotated and a load is applied to it. There are minimal forces on the screw so I think if I am able to find a threaded insert I will go with it.

Furthermore, I am a noob machininst so I think it is also a contributing to the broken taps.


The bar stock is brought heat treated because it is expensive (we found) to send it out to heat treat afterwards from a 3d printing vendor - the vendor prints the specimen, heat treats it and sends it over to us. We are a research lab and we have a few CNC machines in house but we do not have an oven for heat treat/qunching.

THank you so much for your insights.
Click to expand...

If you are stuck with hard tapping in the current configuration, and the alternatives are not feasible for various reasons, then I would buy taps that have *lots* of positive rake AKA "hook teeth" and helical flutes. Maybe the tooling that is meant for aluminum/titanium would work. In any case I would have a long talk with suppliers like Emuge, OSG, and Guhring.

Most of the work I did with Incoloy was for industrial furnaces, and the old timer machinist next door used to use HSS on it. BUT he was turning it OD and ID, not tapping.
 
so the parts have Thor strength. That's pretty tough.
Emugees taps are the best choice. A little pricey. Although not as good, the OSG VC-10 works well and quite a bit cheaper.
Use ;ots of moly-dee or eauiv. If I were hand tapping them, I would fabricate a tap guide to make sure they're going in straight.
Any reason you're not threadmilling them?
 
shyam said:
we have a few CNC machines in house but we do not have an oven for heat treat/qunching.
Click to expand...

" few CNC machines" is a tad vague, Threadmilling has many "votes". If you do not already know their capability, share with PM WHICH CNC machines.

There will be be one or many (I am not among them) who will "know" the machines and if suited to drill and threadmill, same clamping, etc..

After that, less waste motion, more specific guidance, and best of all expectation of good "repeatability".

Page Two:

Research lab and for testing?

If you can afford the investment of "a few CNC machines", you really, really SHOULD look into adding an appropriately sized HT furnace with decent controls and QUALITY instrumentation. Even if too small for half the work, that is still half brought under your schedule control rather than dice-roll.

:)

Even the most helpful of third-party HT contractors will have other demands on their workflow scheduling that you cannot easily predict as but one client of many.
 
You have CNC machines, why are you hand tapping? What are you using for a tapping fixture? What is your hole size before tapping? Use a larger tap drill, the material is plenty strong enough with a 50% thread to break any bolt.

Even if your CNC machines won't do helical interpolation, you can hand code the holes as a series of 3 axis straight moves. I'd start with 30 degree segments if your cam software won't do it for you.

Another bodge that can be a lifesaver is to cut a neck in the tap with a cut off wheel on the surface grinder. Put the neck at the top of the flutes. Start with a neck diameter about 80% of the tap drill size and adjust as necessary. You can purposely break some of your dull taps in scrap material to calibrate the neck diameter to be slightly weaker than the threaded portion. This allows the tap to break leaving a sufficient projection above the surface to make removal easier and doesn't damage the threads.
 
gbent said:
Another bodge that can be a lifesaver is to cut a neck in the tap with a cut off wheel on the surface grinder. Put the neck at the top of the flutes. Start with a neck diameter about 80% of the tap drill size and adjust as necessary. You can purposely break some of your dull taps in scrap material to calibrate the neck diameter to be slightly weaker than the threaded portion. This allows the tap to break leaving a sufficient projection above the surface to make removal easier and doesn't damage the threads.
Click to expand...

LOL! .. and WISE makers of taps have been building that IN for over a hundred years!

Bubba-the-greedy-genius figures them stupid and buys the full thickness versions... of course.

HIS taps won't break any more than his s**t might actually stink to DIN or ANSI standard, after all.

Go figure...

And go thread-mill...
 
You must log in or register to reply here.

Similar threads

R
source for 1/2-13 oversize tap? (for hot dip bolts)
2
Replies
21
Views
1K
Bill D
B
Z
Help! I need to generate a .003R max on the edge of a hole in Inconel 718.
Replies
8
Views
1K
Zeuserdoo
Z
M
Fanuc Oi breaking taps
Replies
13
Views
928
BobM3
B
R
Machining Inconel 625 with ceramics and carbide
Replies
10
Views
2K
Thomas_Brown
T
M
3D Milling With Ballmill/Feed and Speed help
Replies
10
Views
1K
13engines
1








 

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