Questions about rigid taping with a form tap.

I am new to using a VMC and rigid taping and so far the holes I have tapped have been fairly shallow one diameter in thickness. I have a part I am getting ready to program some 1/4" - 20 holes in a 1" thick part the threads will be blind and I want to thread in .500". Should I peck this once or do it in one pass. The material is 6061 T6 the machine has flood coolant. I have been taping my shallow holes at 1000 RPM.
Thanks Mike

Form tapping just do it in one shot no pecking. Form taps aren’t fond of pecking and the momentum of doing it in one shot is actually better

Wind ‘er up and just make sure that your minor diameter is correct and you shouldn’t have any issues.

Greetings.

1/4-20 half an inch deep in 6061? One shot all the way home. With form taps, there's not much to be gained by pecking, since you don't need to clear the chips.
I normally tap pretty much anything under 1/2-13 at 500 RPM, with a 1000 RPM reverse, just to save wear-and-tear on the spindle drive trying to stop the thing and reverse it on a dime. (Big Daewoo VMC. Much mass.)
The 10-15 seconds per run it saves to tap faster is offset by the eventual PITA factor of having to fix the spindle.
Or, at least I own it, and if it fries, I'll be the poor bastard trying to fix it. So I baby it when I can.

Regards,
Brian

2x diameter should be cake. We form tap down to 0-80 3x (sometimes more) diameter routinely.

Thanks for the info prior to this machine I was using a Trak bed mill and a tapping head with cut taps.

We do these at 1200-6000rpm on our Speedios depending on material. 6061 we'll go 3000-6000rpm depending on the exact tap we're using (older taps pulled from the drawer tend to have trouble at faster speeds versus getting a new quality tap LOL). No peck with roll form. Most of our holes are blind and so we form tap just about everything 1/4" or smaller since the spiral flute taps just aren't strong enough in sizes smaller than that (for us).

We have some parts that have tightish tolerance for the hole and thread depth due to breakthrough into other features and we sometimes have to grind the first few threads off a form tap. Those we usually run at 1200rpm or under. Not that we've broken any above that, we just haven't worked up the courage yet!

Every once in a while someone tries to make due with a gun tap in a blind hole and immediately scraps a part from chip packing. *sigh*

Alberic said:

I normally tap pretty much anything under 1/2-13 at 500 RPM, with a 1000 RPM reverse, just to save wear-and-tear on the spindle drive trying to stop the thing and reverse it on a dime. (Big Daewoo VMC. Much mass.)

Click to expand...

So you are cautious of wearing out your Spindle...then you do an instant reverse at 2x the speed? IDK but that seems like it would not help you in that area. You are still doing the same thing (stopping on a dime), but increasing the load on the Spindle by increasing the Speed on reverse. It would follow logic that using the same speed would decrease load on the Spindle.

Whysosharp said:

Form tapping just do it in one shot no pecking. Form taps aren’t fond of pecking and the momentum of doing it in one shot is actually better

Click to expand...

Why are form taps not fond of pecking? What does momentum have to do with it?

Regards.

Mike

gundog,

I regularly go 20mm deep with an M6 form tap without any issues (1000 rpm in a super mini mill).


PM

You don't need to peck even going as deep as the tap will allow, assuming your coolant has enough lubrication for the starting hole size. The more thread percentage you form the more lubricity you need. Spindle speed is limited by your machine, not the tool or process here so go as fast as you want. Coatings are worth getting with form taps, Balax recommends chrome for 6061 aluminum and only charges $1.50-$2 ish for that size of tap with a 1-3 day turnaround since they do that coating in house. I do not understand why form taps are always uncoated as how the tool is used is perfect for a coating.

Rick, Balax makes form taps with 1 thread leads.

I can't back this up with any white papers per say, but I wonder if with pecking form taps, you might run into a bit of work hardening in Aluminum. Especially on larger, course threads, where you're really moving some material around.

Dave

I just ran 50 holes form tapping an M3x.5 thread .4" deep in 7075. 3k RPM. I did one peck just to get coolant back in the through hole. Guhring tap with TiN coating. I don't know if it's advised to peck with form taps in that case but it's on a Speedio and the threads look beautiful.

1/2" deep form tapping 1/4-20 in 6061 should be cake, if the machine is even close to decent.

I just formed a few 1/2-13 holes 3" deep in my little Brother a couple of weeks ago. I did have to buy a Balax tap, since I didn't have one capable of tapping that deep in the box. Didn't have much to hold onto in the collet, but it went like butter. Don't remember RPM, maybe 800-1000. Forming the common 3mm-6mm I do, I run 4000 to 6000 rpm.

litlerob1 said:

So you are cautious of wearing out your Spindle...then you do an instant reverse at 2x the speed? IDK but that seems like it would not help you in that area. You are still doing the same thing (stopping on a dime), but increasing the load on the Spindle by increasing the Speed on reverse. It would follow logic that using the same speed would decrease load on the Spindle.

Click to expand...

1500 / 2000 rpm differential.

How would 2000 be easier on the spindle? Motor? Drive?


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

Think Snow Eh!
Ox

Oddly... I have never seriously considered peck-tapping. Never even tried it.
I have Rigid tapping on both my Haas and Fadal, but I generally use a floating holder on the Fadal as I have yet to tune my gain factors, and the software doesn't que up the Rigid Tap Preparation commands..

I use Blaser 755B coolant these days, but no matter.

But... I rarely break a tap... 10-24 to 1/2" in 6061 at a thousand or so in, 4000 out...
I run that job 4 times a year. About 750 holes. Use the form tap.... never a failure. Never changed the tap.

But if you are worried about the wear and tear on the spindle, there is no way you could beat a tapping head. Not with anything.

But, I got close with a thread-mill.

That job, 1/2" deep.. resulted in oh... I dunno... about 3/8" effective.

I found with this SCT thread-mill.. Punch the hole... dive in with the thread-mill, at 2000 RPM ( Or whatever...) and it goes around the hole just over one revolution to finish the complete thread profile.
And my required effective thread, actually closer to 5/16" was done at constant speed.

Not bad at all, but that is not a cheap mill. I think about $175. for the danged things, and I killed a couple just getting the swing of it.

Anyway... my rule of thumb is just go for it, until something blows.
Then back off 10%

I commonly tap 3/4" deep and more..1/2-13 in mild steel with a common plug tap like Doorman.. heck, whichever one out of the pile cut taps that looked like it might be good.

If I am feeling nervous, I will stand there and brush-on Union Butterfield tapping oil with an acid brush. Or... sometimes.. let the drill cycle go by, blow off the part.. spray tapping fluid into all the holes, turn the coolant off and all holes tapped with oil.

Point is, do not be afraid of failure. " I just snapped a tap and destroyed a part. Shucks."

The loss of a part or a tap is often meaningless unless you are in a repair. ( Depending on value of the target by the time the tapping cycle is applied )

I do love them roll taps.

eaglemike said:

1/2" deep form tapping 1/4-20 in 6061 should be cake, if the machine is even close to decent.

I just formed a few 1/2-13 holes 3" deep in my little Brother a couple of weeks ago. I did have to buy a Balax tap, since I didn't have one capable of tapping that deep in the box. Didn't have much to hold onto in the collet, but it went like butter. Don't remember RPM, maybe 800-1000. Forming the common 3mm-6mm I do, I run 4000 to 6000 rpm.

Click to expand...

That's pretty deep. I was just asked to do M16x2 and 7/8-9 BSW threads in 304 stainless. I'm feeling a thread mill coming on for the 55 degree BSW but the M16 has me feeling frisky...

DethloffMfg said:

That's pretty deep. I was just asked to do M16x2 and 7/8-9 BSW threads in 304 stainless. I'm feeling a thread mill coming on for the 55 degree BSW but the M16 has me feeling frisky...

Click to expand...

In 304, play it safe and thread mill would be my play. I had some 304 once that was the worst ^$%^^ to tap I've ever worked with. If you know for sure it's good material, and you have a good cut tap for it, then go for it. 416, no problem. 17-4 H1150, maybe H1100, no problem. I prefer not to tap H900, although I have done it. (I've had too darn many learning experiences)

Ox said:

1500 / 2000 rpm differential.

How would 2000 be easier on the spindle? Motor? Drive?


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

Think Snow Eh!
Ox

Click to expand...

I'm not following the question.

Well you seemed to be under the impression that M3 1000 to M4 1000 would be easier on the equipment than M3 S500 to M4 S1000.

Now I understand how it's easier on the coder (no need to change the S value) but how are you thinking that it is easier on the hardware?


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

Think Snow Eh!
Ox