Rigid form tapping problem.

I was running some 3/8-24 form taps in 1018 a while back 1/5" deep. On the retract, about half the time I was getting threads ripped out of the top, like 6 threads, so I just went in a bit and had someone finish them off with a hand drill. Fadal, so I blamed the machine.

So now today, on a Mazak, blind hole, same 3/8-24, 9mm drill, .69 full thread depth. First couple came out beautiful. BTW I pecked since all my tear outs had previously been on the retract, I figured the coolant was just getting sparse. Well today, on the 4th hole, the tap snapped on the retract. Slowed the surface speed down from 85 to 60sfm, and on the second hole, I lost the bottom two threads on the tap. The taps were OSGs. I've run 3/8-16 on this machine .5" deep at 1200 rpms and never had a problem.

I know 9mm leaves 75% thread, and the next highest drill will most likely leave my minor diameter too big. Am I doing something fundamentally wrong or are finer pitches just a bigger pain with form taps? A floating head possibly, tapmatics rigid tap toolholder maybe? A different tap, more or less SFM, ream progressivly bigger until I reach my maximum minor diamter.

I'm at a loss, and I am not tapping all of these holes by hand, and I don't think a cut tap is going to be a good choice in a blind hole that deep,

Any suggestions?

My guess would be a lubrication problem. Either that or your drill size may need to be just a tad bigger. Not too much though. Those thread forming taps are picky about the starting diameter. I have used thread forming taps on 1018 a lot, and never had problems. I may also suggest a tin coated tap, or some type of coating that add lubricity. The taps I've used in the past are usually smaller than 3/8 so there isn't quite as much friction. The bigger ones will have a lot of friction, which is why I'm thinking you should maybe use oil. Some kind of moly-dee works the best.

By the way, I do it on my Fadal also, so since you say you've had other taps work fine, I doubt it's the machine.

If you go to a cutting tap, OSG makes good high spiraled taps. They do a pretty good job of extracting the chips out of the hole, so they're not in front of that blind hole.

I think you should go to a letter "T" (.358) drill. I use that all the time for 3/8-24 and the minor still comes in spec. Tapping .69 should be no effort and I agree with Dave, I don't think its the machine. Check on your coolant mix, and double check the hole. Is the hole size shrinking? maybe 'wandering'?

You can cut tap the hole too if you use a hi-spiral cut tap (which will eject the chips out back). The depth isn't that deep for a 3/8 thread. You shouldn't have to use oil either for 1018.

We normally use a "T" drilla s was suggested already. Some coolants just don't work well with form taps, and at least one of the tap manufacturers...I can't remember which one , recommends and EP oil, since the thread are being formed and not cut. Should be able to do many hundreds of holes in 1018. We run about half your speed on the infeed...double on the retract, and use oil...no problems.

Got some new taps in today, greenfields instead of the OSGs(I broke them all), and jumped up to a T drill. My minor is right at the max, I can live with that. No broken taps or torn threads.

Thanx.

I tend to run a lot higher thread % - even in steel. Usually 1200 series tho.

I run my taps a LOT slower than that! A LOT! I don't have much trouble.


Think Snow Eh!
Ox

So, slow, what kind of surface footage are you susposed to run a form tap at anyways? I know, look in the book, its at work though. I can understand limiting the actual RPMs if your machine (Fadal anybody?) gets a little finicky reversing, but, if thats not the limiting factor, how fast can I go?

Bob,
As I mentioned earlier, I have a Fadal, and I tap at 1000 - 1200 rpm all the time. No problems. But also like I said before, I'm usually tapping 6mm taps or smaller. I'd be a little leary of tapping a 3/8 tap that rpm, simply because of the surface area you have rubbing on a thread forming tap. If I were to guess at it, I see no reasong you couldn't go at least 500 rpm.

You said there were some good holes before things went bad. Any chance the tap may be slipping either axially or radially in the holder? RPM seems rather generous to me, also.My old OSG tap calculator shows 25-50 sfm for that size, 250-500 rpm, and sulph/chlor oil. As mentioned, OSG spiral fluted taps would be a good choice IMO.

Well, running 560rpms, 150 holes and the greenfield tap is holding up. The greenfield tap has 4 gashes down the sides on the low spots, the OSG didn't have these, I'm thinking this is letting the coolant in a lot easier, and in turn making my life easier.

Dave, on our Fadal, over about 500rpms, the spindle doesn't reverse fast enough and the part ends up getting pulled out of the vice. Different spindle motors possibly or maybe there is some adjustment I need to make.

Thanx for the help.

Bob,
That almost sounds like you're using a standard G84 instead of the G84.1. If you are using the G84.1, then something is out of wack. Mine takes a second or two to reverse too, but the Z axis still follows it perfectly, and it still only taps exactly what I programmed it to.

Dave, your good, how did you know that I didn't read the entire manual? Your right, I was using G84. This morning (Yes, I'm an idiot and went to work on a Sunday), set up on the Fadal for 1.5" deep 3/8-24, beautiful threads, one shot, 360rpms. I think the Greenfield taps with the big gashes along the side are helping out in getting the coolant in, as opposed to the OSG that had one tiny little slot down the side.

Thanx, that just made my life easier.

Bob,
Glad I could help. You're going to love true rigid tapping. Have fun.