What's new
What's new

Best methods for many threaded holes

I've always thought that chamfering both sides of the hole before tapping would be the preferred method. It's just that it may not always be that easy to flip the part to do it. In this case, being relatively thin sheet it may be. No mention of the actual part size in this thread unless somehow missed it.
 
Thanks again for all the comments - here is where I've ended up:
-Drill from backside (using TSC drill)
-Chamfer (ends up being exit side)
-Flip
-Chamfer entrance and some other features.
-Tap (form tap in this case).

My logic (and I'm definitely listening to those with more experience that I have)
-I want this to run without tool breaks - right now, it's 1 up, but I'll have 6up on the next fixture.
-TSC drill since I'd already bought it, and no issue with 1 plunge.
-Form tap to eliminate chance of chips jamming the tap and breaking it. Seems to work well so far.

Right now, cycle time is loooong - about 45 minutes. I'm tapping at 300rpm, so will look at increasing this. My machine runs in position mode up to 1000 rpm, but I'll ease into it.
I'm happy with the quality with some tweaks to the chamfer depth. No hand work needed.
 
Before you do a million of these make sure your form tapped threads are strong and don't explode in anodize.

Spiral point taps are the way to go here. Form taps are my last choice in 6061.
 
Thanks. That's the next step to work through the finishing process. I'll be ordering some spiral point taps to try as well.
Matt
 
Thanks. That's the next step to work through the finishing process. I'll be ordering some spiral point taps to try as well.
Matt

If you are anodizing be aware form taps crush the material to from the thread peaks. The formed thread peaks aren't homogeneous material. The chemicals used in anodize are very difficult to flush out of the threads. A few weeks after ano the threads in your parts will be full of white powder.
 
Thanks again for all the comments - here is where I've ended up:
-Drill from backside (using TSC drill)
-Chamfer (ends up being exit side)
-Flip
-Chamfer entrance and some other features.
-Tap (form tap in this case).

  • Chamfer backside
  • Flip
  • Drill
  • Chamfer
  • Tap
If the part misloads during the flip, has a chip in the way of the work stop, etc, your tap will be forced to follow the hole done in a different orientation. The machine should be able to put the spindle in the same place repeatably so drill and tap should be done from the same side.

Plus: if the drill didn't penetrate the opposite countersink perfectly, no harm done. Part might be fine, even if 0.010" off position side-to-side.
 
Before you do a million of these make sure your form tapped threads are strong and don't explode in anodize.

Spiral point taps are the way to go here. Form taps are my last choice in 6061.
I dunno, my parts don't get anodized, usually, and I have tapped quite literally millions of small holes with form taps in 6061 and 6063 and get many tens of thousands of holes out of a tap
 
Rivet nuts is a no-go? I have come to love them, bought a battery riveter for these nuts and oh boy is it fast, simple and looks proffessional!

Usually stronger too.
 
That is the best way to ensure no burrs. No extra tooling cost also.

No extra tooling cost but significant extra labour cost. Flipping with a stop may or may not be repeatable depending on who’s doing the flip.

We’ve been running a job like this daily for the past several months, except with more extreme conditions (1” depth, steel, QC gauges every hole on delivery). PITA any way you slice it.

If I had another machine open I would spot the back side deep and let the hole/thread break thru.
 
Thanks again for all the comments - here is where I've ended up:
-Drill from backside (using TSC drill)
-Chamfer (ends up being exit side)
-Flip
-Chamfer entrance and some other features.
-Tap (form tap in this case).

My logic (and I'm definitely listening to those with more experience that I have)
-I want this to run without tool breaks - right now, it's 1 up, but I'll have 6up on the next fixture.
-TSC drill since I'd already bought it, and no issue with 1 plunge.
-Form tap to eliminate chance of chips jamming the tap and breaking it. Seems to work well so far.

Right now, cycle time is loooong - about 45 minutes. I'm tapping at 300rpm, so will look at increasing this. My machine runs in position mode up to 1000 rpm, but I'll ease into it.
I'm happy with the quality with some tweaks to the chamfer depth. No hand work needed.
form taps dont like going too slow, keep it over minimal surface speed.
also if you 100% rigid tap and tapping through other side may snap it due to imperfection of repositioning.
 

About 2 min in to see the speed difference.......
If you can fit this on your machine...........just a thought
Find them on *bay for low money....easy to repair...
 
We had an old tapmatic head back in the day, damn that thing could pop threads in a part so fast, had the bar that slapped back.
 
Last edited:
Yea, I know a VMC can do "spindle " tapping...but to me it just seems better to keep the spindle going one direction.
I base this on my VMC which has to reverse a motor, gearbox, then spindle......lot of metal to change direction, the drive has a lot more work to do than just running a constant fwd speed while tapping with the head.
A Brother or similar machine where the inertia is lower than a "full" size VMC, obviously spindle tapping is fine. .....
 








 
Back
Top