How fast can a VF-2 safely tap?

[TXFred]

This machine has 1000 IPM rapids and a 7500 RPM spindle with a two speed gearbox.

We normally use straight flute taps, plug or bottoming, held in an ER collet. (I know that's not the best way, but it's the only option we have here.)

I generally program slow tapping cycles, 200 RPM in and 400 RPM out. We tap without coolant, using BoeLube paste to lubricate the tap. This means that the operator has to pause after each tapped hole to clean the tap and apply more BoeLube.

I would like to see if I can improve on the speed and also use flood coolant instead of paste.

How fast should I be tapping with this setup?

Frederic

[Geof]

What size tap? What type of material?

On a Super MiniMill I regularly tap 1/4"-20 in 6061 or leaded steel at 1000 rpm using coolant at a mix of 10 to 15%. A coolant concentration below 10% does not give enough lubrication. Occasionally I tap 3/8"-16 and up to 9/16"-NF in hot rolled steel at the same speed but I normally repeat rigid tap in hot rolled.

I also use ER collets and have never had a tap slip. I have broken taps and stalled the spindle but never slip.

[Donkey Hotey]

This is more about material and the type of taps than the machine. Everything about cutting metals still applies to tapping so if you're cutting steel that tears at lower speeds, it will also leave a poor thread finish at slower speeds. In other words, if the material likes to be cut fast, it will also like to be tapped fast.

Generally speaking: try to tap at a programmed speed ABOVE 800-1000 RPM. This keeps the machine in high gear (if you have a gearbox). That taps faster and more accurately. In low gear, the motor has to spin up to higher RPM and it's harder for the machine to slow back down to reverse out each time.

Run your coolant at a higher concentration. I keep the machines at 10% but, if you were doing a lot of tapped parts, 12% will make a difference.

Last: you said straight flute taps. As in, HAND TAPS? There is nowhere for the chips to go. That is just begging for broken taps. If the holes are blind, use a spiral flute tap so the chips will eject out the top. If the holes are through, use a spiral point so the chips will push out the front. If the material is soft (aluminum) consider changing the process to forming taps.

For grins, drill some sample holes in a similar piece of material and try to hand tap using each style of tap. You will be seriously surprised at the difference in force needed between a proper machine tap and a hand tap. Straight flute taps bind up in a few turns from the chips wadding up in the flutes, torque requirements go way up and...'snap'.

[Matt@RFR]

If you're using a HSS tap, then you only need to figure out surface speed for that size...just like a drill. HSS is the same whether it's a drill, tap or endmill. On aluminum, magnesium and brass, I personally go as fast as I can if it's more than a few parts. For example, I make some 360 brass parts with a 4-40 thread, .750" deep. (It's for an adjustment...has to be that deep). I tap that with a Balax form pulley tap with the shank ground to just under the minor at 6000 RPM (not a typo, six thousand) using Blaser coolant at 8-10%. I would go higher on the RPM but the spindle is just getting to 6000 at the bottom of the hole, so it doesn't get any faster. One tap has done about 400 holes and is ready for more.

I also did some parts in 7075 with a 1/2-13 OSG form tap at 3000 RPM with excellent results. That same form tap works really well in 304 at 230 RPM.

ER collets are fine for tapping. The above 1/2-13 in 304 was held in an ER-32 and never moved.

[Ydna]

There was a time a few weeks ago where I had a giant fixture plate to make, and only had some junko hand taps from the "manual" side of the shop. Somebody screwed up on that one.
Anyway the sizes were 5/16-18 and 3/8-16 taper taps, alloy steel workpiece, I did both of the taps at 600-RPM, but I did peck tap the holes. Only cut around 0.050 deeper each pass. I really wanted to experiment given the circumstances but didn't have the time.

All of it made me realize that (IMO at least) hand taps aren't necessarily worthless, but the whole process did take a LOTTTTTTTTTTTT longer having to peck a dozen times each hole. But it at least worked thank god, and the part was delivered...

[TXFred]

Thanks for the replies. My test case is going to be a piece of 1/2" steel plate with a 3/8-16 tap.

Donkey Hotay: Yes, hand taps. We have a few decent spiral point and spiral flute taps, and they've worked great. But we're a manual shop that has recently began to embrace CNC, so we have a lot of hand taps.

Add in the fact that this shop is part of the state government, and it's hard to get money to spend on really nice taps. So we make do, and manage pretty well since we don't have to do high speed production.

I think I will order a nice spiral point tap for my tapping test.

Matt: Tapping at 6000 RPM is not something that I would ever have considered trying. Color me impressed.

Ydna: Oddly, I was thinking along a similar line. Assuming that I don't break off a bunch of taps in the plate, it will make a nice fixture plate when all is said and done. Peck tapping is a good idea too.

Cheers,
Frederic

[TheBigJW]

Emuge has a new versatile tap we have had pretty good luck with for overall performance. we use them in spiral flute to bring the chips out the top.

http://www.emuge.com/multitap/

John