[jheers]

I am having some trouble with a current project. We are drilling and tapping into the top of some steel screws (4135H, as far as I can gather from the manufacturer). The idea is that we will be setting a magnet into the head of the screw, which we have been doing for a little while. The first few parts were made by a guy who is no longer with the company, and he left very little information behind when he abruptly departed. They are socket head cap screws, 5/8-18, and we are drilling into the center of the head, in line with the screw, and milling out a circular pocket in the top, so when the magnet is placed, it sits neatly where the hex wrench would go, protruding just slightly from the top of the head. We have a program that is running, and has run for a while, but we are breaking drills and taps at an uncomfortably fast pace. We run 30 parts at a time; two or three cycles run just fine, then a tool breaks. There is a stop between the drill and tap cycles to make sure the drill hasn't broken. We are running an uncoated HSS 4-40 spiral flute tap and a #38 drill, which is way over the standard #41 drill. We've used carbide drills, but we broke the last one we had, so now it's back to high speed steel. The HSS drill is running at ~75 FPM, .001 ipr (2822 RPM, 2.822 ipm). I just turned the speed on the tap up from ~3 FPM (100 RPM) to ~10 FPM (340 RPM). The drill had been peck drilling, .02 peck depth, to -.875, and the tap was going down to -.6875. I just moved the drill down to -1.125 to make more room for any incidental chips, although it is a spiral flute tap.

That's as much relevant information as I could think of on the spot, so now the real question is, is there something fundamentally wrong with our method (speeds, feeds, etc.)? I have a lot of will, but next to no experience when it comes to this grade of steel. We typically work almost exclusively with aluminum around here. I appreciate any help!

[DareBee]

Instead of peck drill use a deep hole drill cycle (full retract).
Drill breakage is likely due to chip binding
I would be more inclined to run about 200 SFM at 1/2 thou chip load as well.

Get a super HQ tap and how are you running it?
Rigid tap?
Collet?
compensating holder?

[jheers]

The drill is retracting fully between pecks, with plenty of clearance for chips. I can try upping the speed on the drill.

We are rigid tapping. The tap is being held in a collet chuck. The machine is a Haas VF-4. Also, the taps are not, to the best of my knowledge, any kind of HQ taps. I'm not even entirely sure they are the best kind of taps for this grade of steel, but they are the taps we have.

[txcncman]

Socket head cap screws are almost always cold headed and cold rolled. At the bottom of the hex, you can probably see where the broaching pushed material down. This material will typically be much harder than the base material. If I were to try to run this job, I think I would try to take this hardened material out with a spotting drill before attempting to drill and tap. Also, this broached material at the bottom of the hex will cause interrupted cutting, which carbide hates. You will probably have the best luck with cobalt or HSS.

[jheers]

We are spotting first. As I said, it's currently an HSS drill, but the drills we bought in case of breakage are cobalt. I haven't had a chance to run one full cycle since replacing the carbide drill with HSS, so I haven't seen how it runs yet. Since, as you said, the material is likely hardened by the cold working, do you think the tap should be run significantly slower? My biggest concern is that I may be overcompensating and running it too slow.

Now, it is a blind hole, but the drill can run pretty deep and the threads don't need to go very deep into the part, so it is entirely possible to drill extra deep to allow clearance for chips. That being said, I have a feeling that the spiral flute taps we've been using may be too weak to handle cutting this material. Would it be beneficial to use a straight flute tap instead? If so, have any recommendations? I figure a long taper at the end would help, and a spiral point, but should I use two flutes? Maybe three? A specific brand, material, or coating? I feel like I'm really grasping at straws here, so any input is helpful.

[txcncman]

The cold work hardened material will probably be less than 1/16". I would only recommend spiral flute taps for blind holes when chip extraction out of a blind hole is demanded. I would recommend you try spiral point taps and consider tap drilling up to 2 times the required thread depth (or more). Another option might be to consider roll forming taps or even powered metal taps.

[jheers]

I'm looking at three different taps at this point. All three are Guhring brand, one is a powdered metal spiral point plug tap, one is a cobalt roll form, and the third is a cobalt spiral point plug tap, all three TiN coated. I'm really hoping one of these will be the winner.

On a side note, we ran a dial test indicator along the fixture for gigs, and found it was sagging in the middle, which may have had some effect on our drills and taps, so we tore it out and are resetting it with three vises instead of two. I really can't wait for this headache to be resolved. Once again, your help has been greatly appreciated.

[RCaffin]

This may sound silly, but it might work.
Change the hex head screws you are using to Chinese imports. They are generally a bit softer. Since you are not doing the screw up with a hex key, I doubt the drop in strength would be noticed.

Cheers

[juergenwt]

Anneal the screws.

[jheers]

Unfortunately we do not have the resources available for annealing of the screws. Otherwise it would be a reasonable option, since the screws aren't having to meet any demanding load requirements.

[juergenwt]

Put a bunch of screws on the hot charcoal of a grill and let the coal go down or set them heads down on a good electrical hot plate at full power. Heat and turn off.
Otherwise send them to a heat treater for annealing.
Spiral fluted taps are fine. make sure you use a good tapping oil and plenty of it.