Need Help!- Breaking 0-80 Taps.....

[nfrees114]

Hey Guys- So I am tapping some 0-80 Holes .120 deep in aluminum (6061-T6). I am using greenfield taps (same I use on all bigger holes that I tap). Thru Holes. I was running at 3000 RPM and slowed down to 1500 RPM but keep breaking taps. Will do 10-30 parts or so (2 holes per part) then breaks a tap. I am drilling it to .0465 and taking it in steps at .060" per step. Also on my Haas I am retracting at 4x the speed. Any ideas???

[keebler303]

Are you using a form tap? If not, you should be. They are much stronger without the flutes. Also may help to hand apply some tap magic or similar oil. Maybe a drop in each hole prior to tapping would suffice.

Matt

[thedave]

I agree on the forming taps they are great. One thing to remember is they use different drill sizes. I think they are around 65%. Found that the first time I tried to use a .25-20 with a #7 drill and broke a new forming tap. Expensive lesson learned.

[nfrees114]

Thanks for the help guys!! I don't have any form taps but I'll make sure to have some in stock for the next time I have a job like this!! I'll try and limp through this one. I opened up the Hole size from .0465 to .052 and it feels pretty good still. plus the parts are getting coated so i'm sure that'll add some meat in the hole. Hopefully I won't break anymore taps....

Thanks Again for the help!!!
-Nate

[HuFlungDung]

I used to have that kind of grief tapping 0-80 in steel and such. I ordered a package of 1.25mm drills (.049") and have used those ever since. That jump between #55 and #56 drill size is too far, and 3/64 doesn't help any.

[nfrees114]

Originally Posted by HuFlungDung I used to have that kind of grief tapping 0-80 in steel and such. I ordered a package of 1.25mm drills (.049") and have used those ever since. That jump between #55 and #56 drill size is too far, and 3/64 doesn't help any.

so are the threads going to be no good if i use a #55? I did a few parts and put the 0-80 screw in and they seemed ok. plus they are getting teflon coated so I know that will add some to the threads. I will definitly do it different next time but for these parts i don't have time to order taps and drills.... so you use the 1.25mm drills for a normal spiral point tap?

[HuFlungDung]

I use the 1.25mm for all #0-80 cutting taps, but not the thread forming taps, of course.

You'd have to check with your customer and see if the drill you are using is acceptable. It would not hurt to check that your drill is drilling right on the size, and not oversize or you could really get into trouble with the screws stripping the hole. Drilling an oversize hole does not necessarily mean that the screw will feel sloppy, because the sloppy factor is a factor of how much clearance the tap has (H1, H2 etc). But drilling oversize means you are forcing the screw to rely more on its own thread crests to resist stripping out. The more meat you leave in the hole, the more the cross section of the threads in the screw shear zone is heavier and rsists shearing off, aka stripping.

[rschultz@asc]

i was having the same problem not too long ago. went up to a .049 drill and changed to retract at the same rate and its been going good. i was tapping in blind holes with a forming tap.