Would you cut or form 9/16"-12 x 1-1/2" deep, in 6061, with a 7 HP VMC?

Finegrain · Jul 26, 2017

Hi guys,

I have a batch of parts that need a 9/16"-12 x 1-1/2", thru, in 6061. I would think form tapping, but am concerned my ~7 HP spindle will not like that. Anybody with a similar machine done form tapping of this size?

Thanks, and regards.

Mike

Gobo · Jul 26, 2017

My God, I hope a 7 horse spindle would tap that. I use form taps whenever possible.

Jorgo · Jul 26, 2017

Gobo said:
My God, I hope a 7 horse spindle would tap that. I use form taps whenever possible.

I agree. Form tap whenever possible

Sent from my LG-H831 using Tapatalk

MattiJ · Jul 26, 2017

Its about maximum torque and not so much about horsepower. Without knowing what machine you have or your spindle specs the 7hp might be more than enough or totally useless.

Finegrain · Jul 26, 2017

2016 Brother Speedio S700X1 with the 16k RPM spindle. According to the docs I have 27 N-m of torque at 1000 RPM.

Regards.

Mike

MattiJ · Jul 26, 2017

Finegrain said:
2016 Brother Speedio S700X1 with the 16k RPM spindle. According to the docs I have 27 N-m of torque at 1000 RPM.

Regards.

Mike

Was unable to find definite torque specs but it could be 40Nm for std version and 92 Nm for high-torq version.(edit: I am obviously blind since you already mentioned 27Nm)

REIME NORIS | Torque Calculation
Reime-noris tapping torque calculator gives approx 15Nm for around that thread size for thread-forming tap so it seems you are good to go. Thread-forming to steel would be probaly too much.

Milland · Jul 26, 2017

MattiJ said:
REIME NORIS | Torque Calculation
Reime-noris tapping torque calculator gives approx 15Nm for around that thread size for thread-forming tap so it seems you are good to go. Thread-forming to steel would be probaly too much.

Interesting calculator, thanks for the link. I tried it with the following:

14.3mm for tap diameter
2mm pitch
400mm cutting speed (close to 1K rpm)
form tap
.75 machine efficiency (their default)

I got ~15nm torque, but also 18KW indicated power, or about 24Hp. You can still give it a shot, but I'd be prepared for stalling and having to manually remove the tap from the spindle or workpiece from the vise if things go wrong.

[Edited to correct values]

Finegrain · Jul 26, 2017

I get somewhat lower numbers:

Not sure what they mean by, "Resulting indicated power". Seems like a large kW figure for that torque figure.

Regards.

Mike

Milland · Jul 26, 2017

It's the cutting speed, if you go from 400 to 200 mm/m you'll half the power with the same torque load. But you may also fall off the torque peak of the motor, so you'll have to game the numbers to see if you're comfortable with any combination.

Limy Sami · Jul 26, 2017

Finegrain said:
I get somewhat lower numbers:

View attachment 204097

Not sure what they mean by, "Resulting indicated power". Seems like a large kW figure for that torque figure.

Regards.

Mike

Mike
Please don't shoot, because I know very little about form tapping but you do realise that calculator works on metres per minute, which makes your 400 metres / min about 1300 feet / min and 9/16 dia over 8,500 RPM.

Like I said I know very little about form tapping, ......but 8500 RPM strikes me as a ''tad brisk'' for any tapping operation.

Finegrain · Jul 26, 2017

Aack! Limy Sami is right, I got bollixed up with metric <> inches. How about this, for 1000 RPM:

Only 2.6 kW now :crazy:

.

Regards.

Mike

Limy Sami · Jul 26, 2017

Finegrain said:
I got bollixed up with metric <> inches.
Regards.

Mike

That's okay Mike, .....I've been fighting both systems since I left school in 1971, ......and still end up scratching my head muttering ''is that right? .....do it again you silly old sod, .........aah MMMM yea, that's better.''

P.S. your 16.33 Nm torque is 12.08 lbs ft in proper money

Milland · Jul 26, 2017

Limy Sami said:
Mike
Please don't shoot, because I know very little about form tapping but you do realise that calculator works on metres per minute, which makes your 400 metres / min about 1300 feet / min and 9/16 dia over 8,500 RPM.

Like I said I know very little about form tapping, ......but 8500 RPM strikes me as a ''tad brisk'' for any tapping operation.

Hah! Thanks for the correction, Limy, I automatically read it as mm when I should have seen the M.

Stupid metric system, if we had just stayed with furlongs and cubits the world would be a better place...

BROTHERFRANK · Jul 26, 2017

It's the course pitch and depth that is getting me. The material is going to be springing back on the tap and the deeper it gets the more torque is going to be required I believe. I normally would recommend form tapping but I think this application is going to be borderline. You may want to cut tap this one. Your machine also has the full retract peck cycle, G277, available to get plenty of lube in the hole. The through hole helps though, you can use a tap with a lot of lead. A lot of other factors at play too, please post your results and final process if you can.

eaglemike · Jul 26, 2017

If it's a through hole, why not just cut tap?????? Get a tap for Al, that cuts free, and let it fly.
I form tap many jobs, but this one seems to call for a cut tap.

MattiJ · Jul 27, 2017

BROTHERFRANK said:
It's the course pitch and depth that is getting me. The material is going to be springing back on the tap and the deeper it gets the more torque is going to be required I believe.

Yes and no. Most of the work is done probably by the first half inch or so and rest of the tap is just idling along in the hole. Half inch or 2" depth should make not much difference.
(Though Guhring for example recommends forming taps with oil grooves for over 1xD thread depths, like this case. Thread length is only limited by tap shank)

Finegrain · Jul 27, 2017

eaglemike said:
If it's a through hole, why not just cut tap?????? Get a tap for Al, that cuts free, and let it fly.
I form tap many jobs, but this one seems to call for a cut tap.

IME spiral point taps have their limits, for deep threads even of they're through. I have had the stringers pile back up into the hole. 9/16"-12 x 1-1/2" deep is going to make some prodigious stringers, probably 6-8" long.

Regards.

Mike

eaglemike · Jul 27, 2017

Finegrain said:
IME spiral point taps have their limits, for deep threads even of they're through. I have had the stringers pile back up into the hole. 9/16"-12 x 1-1/2" deep is going to make some prodigious stringers, probably 6-8" long.

Regards.

Mike

It's a little over 2 diameters. Not a big deal. Get a sharp spiral point. Or, get a spiral flute and peck tap, Brother machines do that well. Think of cutting 1/4-20 5/8" through - no big deal, right?

Limy Sami · Jul 27, 2017

Just a thought (don't shoot :eek:

) what about thread milling? ........Harvey do them long enough, Harvey Tool - Carbide Thread Milling Cutters - Single Form nice small easily flushable chips, ..............and isn't that the sort of thing the Brother's built for?

gregormarwick · Jul 27, 2017

Finegrain said:
IME spiral point taps have their limits, for deep threads even of they're through. I have had the stringers pile back up into the hole. 9/16"-12 x 1-1/2" deep is going to make some prodigious stringers, probably 6-8" long.

Regards.

Mike

I love form taps too, but I agree with eaglemike that I think I would also reach for a simple spiral point cut tap for that hole.

I don't think it'll be as bad as you are thinking. 3-4" long maybe, not 6-8".

Would you cut or form 9/16"-12 x 1-1/2" deep, in 6061, with a 7 HP VMC?

Diamond

Titanium

Hot Rolled

Titanium

Diamond

Titanium

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Stainless

Stainless

Titanium

Diamond

Stainless

Diamond

Diamond

Similar threads