Tapping speeds?

[sndsa]

Hi Guys,

I have a VF2 with rigid tapping, anywhere I can get some safe tapping speeds for M4 to say M16?

I am still waiting for my tool supplier to give these to me.

I have been using anything below 60rpm, used as slow as 10rpm today (M6),

Haven't had too many problems with M8 and bigger, M4 and M6 snap like twigs!

I only use mild steel and have been using Somta blue ring spiral flute taps (blind holes).

I run edgecam which sorts outs feeds,

thanks

[Geof]

Run much faster than that. I use 1000rpm for nearly everything from 4mm up to 5/8"-18. I have found taps cut better at a good speed. The metal seems to flow easier and form a good chip. Lubrication is also important and I run mine at a 10 to 15% mix which gives better tap life.

Small taps in mild steel a sometimes a bit of a problem and I always try to sneak the drill size up a bit somewhere between 65% and 75% full thread. Repeat Rigid Tapping also helps. Go in about two threads, back out and then go four, then six until you reach your depth. Make sure Repeat Rigid Tapping is turned on in both places in the Settings/Parameters.

[WallyL7]

Haas had a handy dandy little tap speed and feed chart (that I have hard copies of) but I can't seem to find it in the 10 seconds of googling I just did.

But for reference:

6-32 tap in 6061 alum = s2464 f77.0
1018 steel = s1376 f43.0
1/2-13 tap in 6061 = s676 f52.
1018 = s377 f29.

to give you a rough idea of what they recommend.

[txcncman]

Just like drilling, smaller the tap, faster the RPM. In stainless, I have run M4 as fast as 600 RPM. In aluminum, 2000.

[Matt@RFR]

HSS is HSS, no matter if it's drilling a hole or tapping a thread. I've never understood the disconnect on this topic.

[txcncman]

The disconnect probably comes in the fact that there is much more surface contact area and more cutting forces in play with tapping than in drilling.

Also, the average machine with 10,000 RPM spindle is probably not going to be able tap a #4-40 at 10,000 RPM. Ya think?

[Geof]

.......Also, the average machine with 10,000 RPM spindle is probably not going to be able tap a #4-40 at 10,000 RPM. Ya think?

The feed would only be 250IPM so theoretically it should be possible.

Maintaining synchronization during the stop and reverse out may be a challenge.

[Matt@RFR]

The disconnect probably comes in the fact that there is much more surface contact area and more cutting forces in play with tapping than in drilling.

I drill 1018 at 80 SFM with HSS drills. I tap 1018 at 80 SFM with form taps (talk about surface area!) with great results. This is with Blaser coolant at 8-10%, no tapping fluid.

Also, the average machine with 10,000 RPM spindle is probably not going to be able tap a #4-40 at 10,000 RPM. Ya think?

I was hoping some common sense would be applied to my post. Even then, I'm not all that far off of your example in one part I make. 360 brass, 4-40 form tap 2.375" deep.* Programmed at 8000 RPM and my VF-2ss get's pretty close to that by the bottom of the hole.

*It's actually four separate tabs that are .250" thick with 2.375" between the opposing faces. By the third tab, it's hauling ass.

[txcncman]

Most of the machines I work with are a little older with rapid rates at 200 IPM. Just sayin'

[sndsa]

wow I thought my 60rpm was high!

I ran 200rpm with an M6 the other day and broke it as well,

I must investigate the rigit tapping - back and forward etc like you mention, I check my software.

I have the haas handbook, I'll check for the speeds they give.

I also like the idea of going slightly bigger on the holes - I did this with the M6 tap yesterday, tap says go with 5mm, after breaking one I went to 5.2, little loose but its not bad!

[sndsa]

was just given this by a supplier:

speed is 10000 or 16000/3.142/m6 0r m8


feed is =s530*pitch=f


speed 10000/3.142/6=530rpm speed 530 * = 530

so M6 = 530rpm

[l u k e]

Lubrication is also important and I run mine at a 10 to 15% mix which gives better tap life.

I didn't realize that coolant would work for tapping; I've been programming the coolant to shut off then oil the tap on each hole. (What a newbie!)