Peck Tapping ?

[Guyinthedesert]

I'm currently running a job, Cast 718, heat treated. I have some 4-40 blind holes to thread. My first plan was to thread mill them. The thread depth is .225 min and a standard 4-40 threadmill is .175 long. They have longer ones, but the shanks are relieved back, they look so weak it's hard to picture them not breaking. Same thing with grinding back a standard threadmill. Whenever I try grinding one back it's weakens it too much,

 

So, I thought I'd threadmill to .175 and chase to depth. I'm finding it difficult to chase such a small hole in such hard material without snapping the tap off. To add to the problem, my threadmill broke after 5 parts. So here I am on a Sunday morning, and I just finished drilling out all the broken taps. Now I/m looking for a new approach. I thought maybe peck tapping would be the answer. Anybody used it with success?

 

BTW, I'm using both Emuge and Exo-VC-10 taps with Moly-Dee

[metalmansteve]

Can you use a form tap?

[mkd]

how are you producing the minor hole diameter?

 

a buddy uses guhring solid carbide drills without centerdrilling. inconel all day long.

going to the high tolerance of the minor before threadmilling seems to make a difference for him.

 

i would focus on milling to completion....easier said ..

[cincy k]

Do you have a single point thread mill or a full form? You will likely find more success using a single point thread mill at lengths greater than 2xd. Harvey Tool has some 4-40 single point thread mills with a 1/4 LBS. Seems like a perfect fit. Going to the max hole ID is also a great idea.

 

http://www.harveytool.com/prod/Browse-Specialty-Carbide-Cutting-Tools---End-Mills/Other-Specialty-Profiles/Thread-Milling-Cutters_169/Thread-Milling-Cutters---Single-Form_157.aspx

[Guyinthedesert]

Can you use a form tap?

 

I've never tried roll tapping Inconel, but these are also UNJ-3B threads. It's sometimes hard to control the minor dia with form taps

[Guyinthedesert]

how are you producing the minor hole diameter?

 

a buddy uses guhring solid carbide drills without centerdrilling. inconel all day long.

going to the high tolerance of the minor before threadmilling seems to make a difference for him.

 

i would focus on milling to completion....easier said ..

 

I had ordered Guhring RT100HF drills, they are not here (I don't want to get into a carbide salesman bashing rant) I'm using OSG VPN drills with great success. Going larger on the minor seems like a good idea, I'm going to try and ream out one and see.

 

As far as threadmilling, the single point mills I've seen don't look too strong. At $120 or so ea., well be running this job for free pretty soon.

[mkd]

my Buddy indicates all the tools in the spindle to make sure they are running true. also on a production basis he uses Scientific and Harvey Tools for threadmilling. not sure if it is a sometimes or always routine, but he mentioned using a rougher thread mill (used previously for finishing) followed by a newer finisher in sequence. with these tiny threads care must be taken to group these thread mills based on optical comparator results. Yes, same cutter from same manufacturer can have enough variances to effect intersection point from bottom of tool.

over-helping again..

[Guyinthedesert]

Thanks for the suggestions. I opened up the minors to .094, which is right on the high. Made no difference in trying to hand tap them. I'll see if I can find a Harvey TM tomorrow and try that.

[Matthew Hajicek - Singularity]

Are you using the right step-over on the threadmill? I threadmill in hardened H-13. This is my chart:

 

 

For a 4-40 your step-over will be quite small.

[left coast lefty]

I threadmilled a couple of hundred 4-40's 1/4" deep in Ti 4AL-6v with the Harvey and it still looked like new. I think it was 4 rough passes at .005 and a finish pass.

[Guyinthedesert]

Update- I couldn't find any Harvey threadmills in stock yesterday, but I found some Micro-100, pretty much all the same dimensions. I seem to be getting a bit of deflection, but other than that they seem to be cutting good, and they are still in one piece. I did as MKD suggested and I'm using a rougher and a finisher. Good point about checking them on a comarator first, these two were identical, but that woulda been a real ball buster if they hadn't been.

 

I also have some 10-32sti holes, drilled thru and threaded about 1/2 deep. Didn't have any problem with those until I snapped a tap off. I was only tapping them about .35 deep and then chasing by hand. I'm going to try peck tapping these. I'm waiting to get a scrap casting back to try it on.