[apalm]

Need help threading a hole that is probably easy to most on the forum. We are trying to thread a 6-32 UNC .300" deep, and using a .110 drill. Were knew to threading on a swiss and keep breaking the taps. Any advice would be appreciated.

[MCImes]

First, what material are you tapping?
2nd, what type of tap? (roll form, cutting, spiral flute, straight flute, 2or 3 flute, coated or uncoated?)...give us the exact tap you're using
3rd, what machine are you using?
4th, how far into the feed does your tap break? (immediately, half way in, at the reversal)
5th, Rigid holder or floating?
6th, at what RPM are you tapping?

Other things to check:
Double check drill depth before tapping
Double check that the tool holder is on center with an indicator
Try peck tapping? (G83 Z.1 F.03125; Z.2; Z.3)
Ill post more when you answer a few of the questions above.

[apalm]

We got through that job, now having trouble tapping another hole.
-M2
-Were using a cut tap right now thinking of switching to form
-Star SB-20
-Broke one tap deep in the hole, now having inconsistency on the depth
-Rigid holder
-Currently spinning at 300 RPM
thanks for your help

[MCImes]

M2 is tough any way you look at it. although 6-32 should be doable. Did you try peck tapping? Try 2 pecks. Make the first one 60% and the 2nd 40% of the depth. Possibly try 3 if that still doesnt work.

I've had the best luck with a spiral flute cut tap, 3 flutes. Form tapping has higher tool pressure so I doubt you'll have good luck with a form tap in M2.

In general, your tool life is going to be fairly low based on my experience. I'd guess 50-150 parts, probably towards the lower end of that because of the depth. 300 rpm sounds pretty good. You could always try slower just for the heck of it, but cycle time really starts to suffer depending on the volume of parts.

Another thing to try if peck tapping would be to start back further, like Z-.200 then on the 2nd peck the tap has a little time to cool and coolant to get in the hole.

Make sure your chuck pressure is adequate.

Oh! just thought of this, make sure the drill is not work hardening the material before the tap goes in. Make sure you have a small enough peck, low surface footage and ideally High pressure coolant or even better, a coolant through drill. I know they're not cheap, but CT drills help a bunch. At minimum, HP coolant is almost necessary drilling M2 in my experience.

Tapping tool steel just sucks doesnt it. If you really want to pull your hair out, tap a 4-40 in 15V. That stuff goes through taps like popcorn.

[apalm]

Hey man thanks so much for taking the time to help us out, really appreciate it! We ended up doing like you said and peck tapping with a cut tap. Also, like you said the tool life wasn't much (about 50 parts) but we only needed 80 parts for the job. Working in a grind shop, we just bought our first Star about a year ago, and just recently started taking on some more challenging jobs. Tapping has definitely been a speed bump for us haha. Again, thanks for taking the time to help us out!!

[MCImes]

No problems! glad it worked out for you.

Peck tapping has worked well for me when breaking taps becomes an issue. Also, it works well if your spindle doesnt have enough horsepower to tap to depth in 1 shot. The sub spindle on one of my machines wouldnt do a 1/4-20 in 6061 aluminum .700 deep. I had to peck it 4 times! (which seems ridiculous to me. thats not a particularly large, deep or difficult hole to tap...)