What's new
What's new

Deep hole threading? 2x one shot or peck tap?

3DM

Plastic
Joined
Jan 14, 2024
We have a job that needs 400+ 3/4-10 and 5/8-11 holes threaded in 0.75” and 1.50” mild steel.

For the 3/4-10 holes I am drilling with a 16.5mm spade insert drill as I have TSC. (Never used a spade insert drill before) Using a spiral flute tap, I don't see an issue tapping the 0.75” plate in one go, but on the 1.50” depth hole I am not sure. Thinking G84 peck tapping to help the tap last. Never tapped holes this large.

For the 5/8-11, .539 carbide drill with TSC, spiral flute tap, straight through the 0.75” but again on the 1.50” material wondering if peck tapping would help the tool last.

I can speed up the retract with the 130 settings, I have done that before. But never used the G84 cycle before. Of course the battle of speed vrs tool life. No idea how long the taps will last, I just don't have the experience with this size tapped holes in mild steel. Sure don't wish to brake off a tap.

Machine:
2022 Haas VF2SS

Any suggestions? Depth is no issue, just run it? Using G84 maybe it causes extra ware since it’s touching the threads 3x or 4x?

I appreciate it.
 
Based on you're wording I'm assuming these are through holes? If so you should be using spiral point taps, those should have no trouble driving all the way through either of those holes.

Either way you're only at 2.5xD on these threads so as long as you're running a nice spiral flute tap aka an OSG or the like it should have no issue tapping them in one shot. Just make sure you tap it fast enough so the chips fling themselves off the tap.
 
Based on you're wording I'm assuming these are through holes? If so you should be using spiral point taps, those should have no trouble driving all the way through either of those holes.

Either way you're only at 2.5xD on these threads so as long as you're running a nice spiral flute tap aka an OSG or the like it should have no issue tapping them in one shot. Just make sure you tap it fast enough so the chips fling themselves off the tap.
Yes through holes.

Good point on the chips with speed. They will be some long stringy things for sure.

Thank you.
 
@3DM
I'd look into thread milling.
Especially on larger threads - say those over 1/2" - as it places much less strain on the spindle and drives. Long life and great control over the thread size.
I originally thought to thread mill but most of the thread mills I see are 1.25” in length. With that 1.5” material I would probably have to go to a 3x the cost longer reach tool. So set up the first run to use the spiral flute taps.
 
Yes through holes.

Good point on the chips with speed. They will be some long stringy things for sure.

Thank you.
Then I'd for sure go with spiral point taps. They're stronger and you'll have better chip control. I like Emuge multitaps but any decent one should work for what you're doing.
 
I was going to suggest form taps until I saw the machine you are running it on. On a 40 taper Haas without a gearbox, you would probably stall it with the 3/4-10. It still might be worth it to try on the 5/8" though.

With a form tap you don't have to worry about chips at all, and 1 tap will easily do all of your holes.
 
Well now, here is what I do. If it was a standard depth of a diameter or or one and a half diameters, so what?
But, now, think about it. If you have 1 1/2" inches of thread in the hole...
Why go for an 85% Thread form?
It gains you absolutely nothing.
CHEAT!
Go with an oversized tap drill, be happy with a 65% thread. You make up in just sheer quantity of threads and engineering WILL bear this out.
 








 
Back
Top