What's new
What's new
By:
Advanced search…

Deeper tapping on a VMC

doug925

doug925

Titanium
Joined
Nov 21, 2002
Location
Houston
I need to tap through some 2" thick A36 plate.
The tapped holes are:
1x8, 24 times
3/4x10, 24 times
1/2x13, 12times

Now I know you are asking why I am bothering to ask this huh?:willy_nilly:
Well, this presents some tricky situations.
Most spiral point CNC taps are not necessarily long enough to tap through 2" of material.
I am afraid of using "pulley taps" as they are weaker then $hit, and I've never had good luck with them.
I am trying to NOT have to finish these by hand. (oof!)
These holes go in some 19" diameter steel plates, so processing by hand won't be too much fun. Neither would any unnecessary handling.
This will be done on a 12 hp Hurco VMX24 with high torque.
All the taps will be run in tap collets, in ER45 holders.

I called Vega-tap to get their recommendation. I quote "... well THAT is tricky. I am not sure what taps you would use. I'll get back to ya. "
Well heck, I need to order these today.:(

What say you group?
Should I be looking at another brand?
What about peck tapping depths?
What will the extra depth do to my SFM's?
Should I be thinking forming?
Can I really expect a 1/2x13 tap to make it through 2" of material 16 times.

Thanks,

Doug.
 
The 1 inch and 3/4 I dont see much of a problem if you go nice and slow and peck tap. The 1/2-13 may run smooth if you use a 1/3-13 nut tap. It has an overall length of 7 inches and the thread length is 2.5 inches. The first 1.25 inches at least is chamfer. The shank is smaller than the minor thread diameter. I am not sure if this will work or not, just thinking out loud.
 
Definetly think forming on the 1/2 tap would be the way to go

the 1 and the 3/4 tapping, go slow.... use a through tap if possible(way stronger than spiral) and progressively peck tap the holes with plenty of cutting oil

Also how much torque does your hurco put out at the rpm reccomended for the tap and how much torque/power does the tap take to turn in that material.....because if it takes 300 ft/lbs at 200 rpm and your machine puts out 100 ft/lbs at that speed , you could be in for trouble*

Boris

* been there... stalled the machine... played with the setting, done the job and scrapped the spindle afterwards :eek:
 
I see no reason that a spiral point shouldn't be used here?

A pulley type on the small one ... but ???



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

Wake me up early, be good to my dog and teach my children to pray.
Ox
 
Have you thought about thread milling? It is slower, but you get a good thread and you don't have to worry about digging out broken taps.
 
The 1" and 3/4" shouldn't be a problem, just use good spiral-point taps.
For the 1/2", can you 'cheat' a little and use a .437 drill instead of the standard .422?
This reduces torque, and helps tap life considerably.
 
Doug, I know we have run 3/4"-16 thru 1-3/4", and don't think that there would be too much problem with 2" deep...just run your coolant a little rich and make sure you're down on the bottom side of the sfm range. The 1"-8 shouldn't be an issue for length either, just not sure how much shank the ER collets are going to suck up. For the 1/2"-13 (and 3/4-10 if you so choose), quite a few (Hertel, OSG, Greenfield, etc.) make extended reach gun taps...those should work fine, just make sure you are getting a nice set (same number as flute count) of dredlocks coming out of the bottom of the hole.

Let us know what you end up using.

Steve
 
I decided to go with OSG's 917 line of extended gun taps for the 1/2x13.
A standard cnc style Vega spiral point tap for the 1x8, and the 3/4x10's.

NOW, I am worried about the torque needed to drive the 1x8.
Since Boris was so nice to point out that I should check the torque needed, Vs what my Hurco has, I am a bit worried.

Hurco can not tell me what that torque curve is on my '06 VMX24HT (high torque 8K rpm)
The brochure says 105ftlbs @ 600 rpm (I am guessing peak)
BUT, no other info as to describe the curve. Corporate gave some #'s that don't make much sense, so I am not sure what #'s to use.

Also, how do you figure torque for tapping?
I was able to locate formulas for turning, drilling, milling, but not tapping.
Since force required for a cut is in direct proportion to feed per tooth, and tapping the feed is set, how do you calculate it?

Thanks,

Doug.
 
I tapped some 1x8's on our old 1991 BMC 20. I set the RPM as low as it would go, which I think was 100RPMs. I put some of the nastiest but most effective tapping fluid I could find it was Energy Release brand. The machine tapped through about 5/8-3/4 inconel fine for the first couple dozen parts. Then the tap started dulling and the machine stalled. Guess what I did....??:D Need more torque how about momentum...? I cranked the RPMs up. Several times... as the tap got duller I needed to run more like 150RPMs... Kick arse man! you should of seen the billows of smoke from the baby machine as it rammed that tap through the hole! Maybe this will help you a little with figuring your machines limitations. My guess is you have plenty of torque if you have the nads to crank the Rs up to meet your torque curve. I don't know if you may have the same torque rigid tapping or not, as the spindle is forced to accelerate from a dead stop. I guess you could call a higher clearance plane to let the spindle wind up to speed before entering the hole. Maybe this helps?
_Greg
 
A sqr drive socket on a trq wrench will tell you how much trq it takes - at least as static. The trq requirement may go up a bit at speed. ???

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

My best friends are flakes.
 
I'd call OSG and see what they reccomend, they have got me out of a few jams.

On several jobs with long thread lenghts that have given me problems and did not have much luck or the time to request help with, I have "Necked" the backside of the tap. That is, grind the backside of the tap leaving only several turns of full thread on the tap. My thought is less friction due to less contact while allowing more coolant / tapping fluid to hit the cutting area. Maybe mind over matter, but I have seen a reduction on the spindle load meter and made it thru the job in many case, not all but many. I have tried with good results on both spiral point and spiral taps.
 
So according to the chart linked to by Scott,
(if I did my math right) then by using a helical flute tap in material that is 220BHN, then my torque should be @ 37ftlbs?!?? Cool!

Thanks,

Doug.
 
You must log in or register to reply here.

Similar threads

3
Deep hole threading? 2x one shot or peck tap?
Replies
7
Views
693
Matt G
M
E
What is projection on a tension and compression tap holder?
Replies
5
Views
267
EyeEmTrash
E
MillGuy88
Issues with spiral flute taps
Replies
4
Views
285
MillGuy88
MillGuy88
W
getting a snug fit end tapping aluminum extrusion
Replies
7
Views
302
edwards.a
E
M
Best methods for many threaded holes
2
Replies
36
Views
3K
MwTech Inc
M








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top