Tapping and threading 3-48 holes

I need to drill and tap 50 holes in mild steel with 3-48 thread. The blind holes are drilled to a depth of .25" and I'm trying to get about 3/16" of thread depth. I drilled four test holes with a 5/64th (.078") drill bit and subsequently broke taps in two of the test holes. I started with a taper tap which worked well but bottomed out after just a few threads. I followed with a plug tap (3-flute) which broke toward the bottom of the hole. I enlarged the next test hole to .081", used plenty of tapping fluid and used compressed air to blow any chips out but still managed to break the plug tap. I was only successful with two of the four holes (I had no issues using the bottoming tap). Any advice on how to tap these holes successfully would be very much appreciated.

Use a form tap

I don't know what your level of experience is, so forgive me if this is obvious:
-- Countersink chamfer the hole before tapping. 10% over the major diameter is good.
-- Use a spiral point tap to initially tap the hole. They are so much better than the other types because they self-clear the chips, even though the chip is left in the hole. You can get it out with air blast usually, sometimes the chip comes out with the tap when backing out.
-- Make sure the tap is straight to follow the hole. (tapping block?)
Mild steel is kind of a pain to work with in most cases. It often has hardness variations (hard spots, inclusions, etc) that make it more difficult to work than it should be.
Another approach might be to form tap the holes. I have never used form taps in steel, but they work very well for me in aluminum for getting threads down to the bottom. Different hole size required.

I've used grease on taps to catch the chips in the flutes when doing auto work such as installing keenserts/timeserts into places like oilpans and transmission housings. Maybe that's an option here with your bottoming tap? .02

I like to use spiral flute taps for blind holes because they eject the chips out the hole and make breakage of the tap less likely if the hole size and the cutting fluid are suitable. Spiral point taps are perfect for through holes, but a pain in a blind hole unless you can drill much deeper than the tapped depth and leave the chip in the hole.

For high quantities, I have had very good results with a Tapmatic 30 TC/DC head in my vertical mill. It is quick and accurately controls the depth. You need a fixture to hold the part in place so the tap lines up with the hole, possibly just your vise and a stop. For lower quantities, but more than two or three holes, I use a Phase II copy of a Lassy tapping tool and am very happy with the results. This device makes it easy to control the tapping depth by counting turns of the hand crank. It is slower than a Tapmatic, but far better than a hand tap wrench. Both of those methods assure the tap is perpendicular to the work, which is vital, but especially so with small taps.

Larry

IME there are 3 big factors in tapping success,

1) tap quality, what are you using?
2) hole quality/location, are you sure your tap axis is concentric to the hole and it's on size?
3) chip evacuation, whether the chips go fore or aft do they have the space to do it?

Programmed via Mazatrol

Are you using Moly Dee?

I had to tap a bunch of 2-56 holes in 1020 mild steel. I was breaking about 1 per part (16 holes) even with tap magic in one of those hand powered alignment fixtures. I got frustrated and made a fixture for my CNC mill. I proceeded to tap over 900 holes without one broken tap. Absolute consistency in torque and rigidity can make a huge difference. This was on Doosan DNM 5700.

EDIT: Used a Techniks rigid tap holder.

Another vote for spiral flute, or form tap. Calc shows .082 for a cut tap.

'Mild steel' can be nearly anything, all the way up to pure garbage. I'd honestly be more comfortable doing those in 4140PH.

I would offer one more suggestion. With a #3 tap, it is awful easy to apply too much torque and awful hard to feel the resistance when the chips start to pile up or you hit a hard spot in the steel.

Whenever I tap holes smaller than #4 I switch from using a tap wrench to using a PIN VISE. The pin vise has a much smaller diameter than the length of the tommy-bar in a tap wrench and it gives you much better feel and control. It is also a lot easier to keep the pin vise aligned with the hole as you are not constantly letting go of the tap wrench and grabbing it again. You just remove the thumb and fore finger while the swivel at the back end of the pin vise remains fixed against your pawn. In fact, it is actually faster than using a tap wrench.

Yes, the tap can slip in a pin vise, but that is not a bad thing. In fact, it is a very good one. When that happens, I back out and clean the chips from the flutes. Dip the tap in the tapping fluid again and continue tapping.

And yes, a guide block is a very good idea. And definitely use a good tapping fluid; one which lubricates. And the chamfer at the entrance to the hole is a must. All good ideas. But the pin vise is the really good one.

If the tap drill is longer than the tap, and the machine is a little out-of-tram then the tap may be under stress for off location..

Freehand/eyeball tapping 3-48 can be a big mistake.

Are you tapping a flat or on a diameter? if by hand, how are you assuring your straightness?

One way to assure straightness is to put your tap drill in a tap holder and with it in the drilled hole eyeball past the drill to something that is straight and square, then do your tapping for that hole...but setting up in a drill press and having the tap holder supported by the drill press spindle is much better than freehand holding the tap wrench.

A 48 thread will advance about .021 per turn so to go 3/32 you need about 9.4 turns, plus add whatever number (distance) of threads is in the tap lead...so to be sure you don't bottom out.

wesg said:

'Mild steel' can be nearly anything, all the way up to pure garbage. I'd honestly be more comfortable doing those in 4140PH.

Click to expand...

Good point.. There are times when a job calls for "mild steel" and A36 would work just fine, but much
better off buying 1018 for a bit more money, just to make the job go easier..

A36 is a crap shoot, sometimes its just so sticky and gummy. It'll mill fine, it'll turn fine, but
I've had some batches that I couldn't do anything that involved drilling a hole, or tapping that
was consistent, or easy.

To all who replied: You guys are great and I'm lucky to have gotten your input. Thank you.

MJT/Wesg/Specfab: I've never tried a form tap. I'm going to try that.

Specfab: Chamfering the hole before I tap it is how I should have started. Wish I had thought of that myself. Also, the taps that I broke were straight fluted, uncoated, steel taps. I'm going to order some spiral pointed taps. I'm tapping on a mill, using a short piece of steel with a ground point. I hold it in my drill chuck and center the pointed end in the top of the tap wrench to keep the tap aligned. It is not spring loaded so I have to keep lowering the spindle every few turns. I do have a spring loaded tap guide so I think I'll switch to that.

Cole2534: Of the two plug taps that broke, one was a newish Cleveland and the other was much older but I can't read the brand name. Your point about using quality taps is appreciated.

Terry: I've never used Molly Dee before but I see it is highly rated. I'll try that.

EPAIII: Yeah, the heart of the problem is too much torque on a very small tap. I've used smaller taps before but they were in aluminum and cast iron, not steel. Your suggestion of using a pin vice instead of a tap wrench should help. Thank you for the link to McMaster-Carr.

Michiganbuck: I'm tapping a flat surface and assuring straightness with a pointer held in the drill chuck of my mill. If I'm still having problems after trying some of the above suggestions, I'll switch to some type of tapping block.

For anyone who might be experiencing the same issue (breaking small taps), I thought I'd post a follow-up about what worked:

By far, the best recommendation was to use a forming tap with Molly Dee as a lubricant. I also used a spring-loaded tapping guide mounted in my mill chuck to keep the tap perpendicular to the work surface. I bought an OSG 3-48 cold forming bottoming tap. I had no previous experience using a forming tap but the advantages are numerous. The tap drill size increased from .078" to .089" (65% threads) which meant the torque on the small tap is significantly reduced. Since the forming process does not produce chips I did not have to constantly reverse the tap to clear them. Since it was a bottoming tap, I didn't have to use two different taps to complete the threads in the blind hole. It was very obvious when I reached the bottom of each hole which reduced the likelihood of tap breakage. Finally, Machinery's Handbook notes, "The threads thus produced are stronger than conventionally cut threads because the grains in the metal are unbroken and the displaced metal is work hardened."

My second choice would have been to use a spiral-fluted tap. I bought one (a plug tap) and tried it out. It produced a nice, unbroken chip that emerged from the blind hole as I turned the tap. However, as I got deeper in the hole, the torque increased somewhat and I was worried that I'd break the tap. At that point, I switched from a tap handle to a pin vise but the shaft of the small tap tended to spin in the aluminum pin vise collet so that method didn't work out for me.

Chamfer.
Use a semi-bottoming spiral flute tap from a respected manufacturer.
Use a tapping head with reliable torque control.
If you dialed in the holes using the DRO dial in the tap locations the same way too assure an accurate location.

Bobw said:

Good point.. There are times when a job calls for "mild steel" and A36 would work just fine, but much
better off buying 1018 for a bit more money, just to make the job go easier..

A36 is a crap shoot, sometimes its just so sticky and gummy. It'll mill fine, it'll turn fine, but
I've had some batches that I couldn't do anything that involved drilling a hole, or tapping that
was consistent, or easy.

Click to expand...

For what it's worth, I have found that when a job calls for mild steel 44W always machines
better (more consistently?) than A36. Not all suppliers will carry rounds and flats in 44W but
it is available--sometimes you just have to specify the material. Where possible I've also had
blanks of 44W cut from plate as well. A bit more cost but to me it's worth it to get a better
quality material...

Perhaps I should have mentioned that I have not tried using a forming tap in a pin vise.

FWIW I hate spiral flute taps under 4-40. There is just no strength in them at all. Any slight irregularity and it will break off.

On smaller taps I almost always form tap. If a form tap won't work I plug tap and then chase if necessary.