fear of tapping

[motodog]

I've got to tap several blind holes in 6061 -t6 and have decided to try thread form tapping to minimize the chip issues. Its a 8 x 1.25 thread and it seems like about .295" drill size should do it. But I'm pretty clueless about feed speeds, and whatever else I'm clueless about (how could I know?). I'm using rigid tapping on a haas vf0 with a floating toolholder. In the past I have put about 1/2 the thread depth with a conventional rigid tap and hand tapped the rest, but in the interest of avoiding carpel tunnel.....I want the haas to do the work!

Any tips or experience would be appreciated.

 

Thnx

[Jack Mitchell]

Hey motodog,

 

Loose the floating tap holder - you'll be glad that you did.

 

 

Just lock it up with a collet and call it a day.

 

 

Regards, Jack

[motodog]

Im scared...waaaa

[motodog]

Ok, so I lose the floater. Other than that, just pound it in? I've never used a threadform tap. Hence the abject fear.

[JazzBass]

motodog,

 

I have had trouble rollform tapping bigger sized threads on my Haas VF-0 due to lack of torque. I never use floating tap holders when I rigid tap. I rollform all blind holes, and cut tap thru holes. It works out great. Don't use the same sized drill for cut tapping!

 

Is your program inch or metric?

[motodog]

Its inch, but I convert from metric

[Jack Mitchell]

The form tap will require a larger tap drill.

Please consult Machinery's handbook for the exact size. Sometimes the correct size is stated on the tap as well.

 

Fear not - just blow it off right to .03" of the drill shoulder - piece of cake, don't ya know!

 

Regards, Jack

[kccadcam]

.295 hole is correct.

Drive it home at 1000 rpm and .0492 per rev.

Solid holder.

Push go and duck!!

[JazzBass]

Use a 7.4mm drill,

 

Here is the feed and speed I would use.

 

S508 F25.

[kccadcam]

quote:

---

S508 F25.

---

Why so slow??

I thought I was being conservative...

The Balax catalog recommends 100SFPM for form tapping aluminium...

[Lars Christensen]

Can someone inlighten me in thread formers, why use them insted of cutting taps?

 

Lars

[JazzBass]

Lars,

 

No chips, stronger thread due to compacted material,

 

You must really watch the minor diameter though!

[Psychomill]

Roll form is a piece of cake. I think .295 is bit big on the drill though. I use a .290 (letter L) drill for M8. If you use a .295, make sure to check the minor diameter to see if its in print.

 

Hole sizes for metric thread are an easy calc. For a cut tap, you subtract the pitch from the major dia of the thread. For roll taps, you divide the pitch by 2, then subtract that from the maj dia. For example, we'll use your M8 x 1.25:

 

8-1.25 = 6.75 (hole for cut tap is .265)

 

1.25/2 = .625, 8-.625 = 7.375 (hole for roll is .290)

 

If you're more comfortable with a cut tap, then you could use a spiral fluted cut tap in the blind hole. That way the chip comes out the back of the tap instead of being pushed down like a normal tap.

[connormac]

Motodog,

 

I agree. solid holder. S508 F25. . Watch finish hole size after tapping. Should end up around 6.75mm.

[JazzBass]

Kevin,

 

That's the scared feed and speed!, for prototype.

 

For production, S1524 F75.

 

I know for a fact our VF-0 will not handle the later.

[Lars Christensen]

So the material and size is you limit for choosing ?

[motodog]

Hey, thanks all. I know that like most stuff, once you do it, no worries.

 

Luckily, I'm the QC guy here also (one man shop), so I've never even used a thread gauge. Just rattle the bolt......

[JazzBass]

Lars,

 

The only time I cut tap are in plastics and thru holes. I rollform 2024 al, 6061 al, 7075 al, 1018 stl, 303 sst, 304 sst, A2 stl, 416 sst, 440c, and titanium.

 

Roll form tap break less often too.

[?Mark]

quote:

---

Can someone inlighten me in thread formers, why use them insted of cutting taps?

---

For one, never broke one (yet)

 

For M8*1.25 use .2913 or "L" drill and no worries.

Will run forever in alum.

 

Kind regards, Mark

[motodog]

Thats what I've heard Rick.

I've had good luck tapping in the past with this vfo, but I've always been really careful.

There is no room for chips on this part, tho. So I figure that roll form is safer.

[CNCme]

Good Day,

 

If there is not much room, you might want to

blow out the holes before tapping.

 

Tony G

CNCiT Precision Machine - Hudson,NH

X Beta Site

Almost Employed Senior Programmer

N.E Massachusetts - Southern New Hampshire

_________________________________________

End mills and tooling are like The "AMMO"

And coolant and chips are like the enemy

Under your boots as you advance in the

Manufacturing Battle

--------------------------------------------------

[motodog]

Thats what I'm really looking for...the voodoo.

 

Science is easy. Voodoo is hard. Thanks. I also intend to hand lube, no coolant, unless someone can convince me that the Kool Mist coolant will do it.

[?Mark]

quote:

---

I also intend to hand lube

---

Why not use a coolant? (I always do.)

Do not try to run it dry, alum will stick to the tool and ruin it propably on a first hole...

 

Kind regards, Mark

[MetalMarvels]

ABSOLUTELY don't run it dry!!!!! I rigid-tap roll-form all day (and night) at 1200 to 1600 rpm on the smaller taps in 6061 with flood coolant at about a 10% mix (Blasocut 2000SW). On an M8 tap I usually run about 1000 rpm. Use a hard collet (no floaters). The upper limit on my equipment is about 1800 rpm - at 1900 rpm it loses synch and "drills" the threads. After about 6-10 holes of "drilling" it - the tap gets partially left behind. I guess form taps arent really very good as reamers. Be aware, the "faster" you tap, the more "headspace" you need at the bottom of the hole to handle overshoot (I am talking about a Fadal here guys!!). For some reason, taps don't like to be smacked into the bottom of the drilled hole........

 

BTW - the first couple of holes with small taps still makes me cring waiting for that gut-wrenching little "pingggg-scritch".

[Müřlıń®]

Hammer down, no guts no glory.....heh....

 

800 RPM in 420SS 1/4"-28 1-1/2" deep of actual thread. Relieved a standard tap with a lathe tool in the collet of the mill so it would go that deep..

 

390 blind holes took a couple hrs for me to do on a mini drillpress with a motor-reversal micro switch on it. Ganged parts 5 at a time in a Kurt that floated on the drillpress table.

 

'bout a second a hole...

 

brush with oil......

 

Only broke 2 taps......

 

 

Murlin teh old school.....