Tapping advice

[ISHY]

Hi

I am trying to tap some M2 blind holes 6mm deep into 6082T6 alli. I have tried a tap at the correct spindle speed but the taps consistantly break after doing 3 or 4 holes. So I switch to thread forming, the recommended speed for the thread former is 3000rpm and this broke in the first hole. I am now having a new one delivered, the manufacturers recommend 6000rpm, I will try this tomorrow.
My gut feel is that these spindle speeds are very high (this is ridgid tapping) I am confident that the machine is up to the job as it's only 2 years old but it seems to me that when it bottoms out and reverses direction 6000rmp is just too fast. The hole I have drilled is 1.8mm and is 7mm deep, is this deep enough or do I go to 8mm (can't go anymore than this).
I have done many successful tapping cycles before be never as small as M2.
Any tips or advice would be greatly appreciated.
Thanks
Ishy

[PixMan]

What machine & control are you trying to do this with? Even with rigid tapping, a lot of machine manufacturers are overly optimistic about the speeds with which you can do rigid tapping.

For an M2 on most controls, you'd be wise to stay under 2500rpm for a tap that small. There are a lot of machine parameters involved in setting up rigid tapping cycles. Most machines do not have any user adjustments for times it takes to stop the spindle at a given RPM, the time it takes to restart in reverse, and the time it takes to to get back up to speed. In all the time it takes to do this (and we're talking about less than a second), the mismatch of rotation to movement could easily snap an M2-size tap. Slow it down, your chances will be better.

[HuFlungDung]

I think it would be a good idea to watch the Z axis depth while allowing the tap to 'cut air' at whatever speed you are experimenting with. If the machine coasts an extra mm before it reverses, then you have to allow for this with your drilling depth and with the commanded tapping depth.

I like to grind off the pointy end of the small taps, just to gain that extra safety space.

Tapping in high gear is probably better too, because the spindle motor won't be spinning as fast. This makes a noticeable difference on a Haas, in how quick the tap reversal occurs.

If you cannot find spiral flute taps in that tiny size, you may end up using 'plain taps' and these are sensitive to chip buildup. You might need to step tap the hole, just to permit lubricant in properly, and the chips out. For comparison, I tap a lot of blind #0-80 holes about 4 to 5 mm deep and always step tap. Hand tap a few holes to gain a feel for how well the tap is cutting, and how far you dare go before backing up.

[ISHY]

Originally Posted by PixMan What machine & control are you trying to do this with? Even with rigid tapping, a lot of machine manufacturers are overly optimistic about the speeds with which you can do rigid tapping. For an M2 on most controls, you'd be wise to stay under 2500rpm for a tap that small. There are a lot of machine parameters involved in setting up rigid tapping cycles. Most machines do not have any user adjustments for times it takes to stop the spindle at a given RPM, the time it takes to restart in reverse, and the time it takes to to get back up to speed. In all the time it takes to do this (and we're talking about less than a second), the mismatch of rotation to movement could easily snap an M2-size tap. Slow it down, your chances will be better.

This is exactly what I think, my gut feel is to do it slow say 500rpm as I'm not in a hurry but all the Reps keep telling me if I do this the roll tap will be more likely to snap but I've run lots of other larger roll taps at this speed ok.

[Caprirs]

I routinely run small roll/form taps into aluminum on my machines. Typically 0-80, 1-72, & 2-56. I never exceed 1000rpm because the threads get measurably bad at higher spindle speeds when checked with a thread pitch gauge.

For a 2-56 thread .250" deep minimum full thread, I peck drill .078" dia x .300" deep, then rigid tap to .275" deep.

Have you tried adding a small dwell at the bottom of the tapping cycle? My Mitsubishi controls support a P value which assures the spindle and Z axis are both stopped at the bottom before reversing.
G84 Xx Yy Zz Rr P(dwell) E S

[rk176]

Ive taped a few thousand M1 M2 holes in my time. My advice would be to keep the speed down to around 750 revs and only tap to half depth till you find out how good the machine is at repeating.If cycle time allows I would just start the hole on the machine then Handtap to depth this save time and taps

[ISHY]

Success, ran it at 800 rpm and no problem at all. It annoys me that the makers of this roll tap tell me to run it at 6000pm but sorted now so thanks for all the help.
Ishy.

[boognish75]

My experiences with tapping any type of aluminum thus far has been to feed in slow steady evenly in and out using a decently thick tapping oil, it appears that aluminum likes to gunk up on the tool and its self due to its soft mallability.

[PixMan]

Originally Posted by boognish75 My experiences with tapping any type of aluminum thus far has been to feed in slow steady evenly in and out using a decently thick tapping oil, it appears that aluminum likes to gunk up on the tool and its self due to its soft mallability.

Material build-up of aluminum on HSS taps is a problem, and worse when the taps are TiN coated. That's why I've always had much better results using Balax Thredfloer BXDIECAST taps made of powered metal and with their Bal-Plus high-lubricity coating. They're also made for CNC work, with the tip removed and lead reduced to 1-1/2 to 2 threads.