fear of tapping

[one shot]

Die thread Die

[CAM-mando]

Moto,

 

I always use inch per rev feed rate when rigid taping on our machines. No need to change feed rates when changing spindle speed. I am not familiar with HAAS though.

[Chris Rizzo]

Spindle speed over ride on Haas is disabled when in G84, as is feed hold. I beleive it's default if rigid tap is enabled. I don't have a setting on any of our pre 01' machines to change that.

 

m2c.

[MetalMarvels]

Someone needs to change the inserts on this threading die, they must be getting dull by now - DIE Thread, DIE!

 

I rather prefer the Vegaroll taps myself (bright - uncoated) for aluminum, but I have had good use out of several other brands. Usually thousands of holes with full flood coolant at about a 10 to 12 percent mix.

 

 

O.O just noticed - 500 posts!!!!!

[Lars Christensen]

Tried my 1st. form tap, actually 2 of them. a M1.6 and a M4 in 316L SS, 1st. time ever worked in this material, and I don’t like it so far. I have some problems determent what SFM and CPT to run.

The parts has 8 M1.6 and 4 M4, the form taps are working great so far (SFM 45 with Hy-Pro Tin coated), but my drilling is giving headaches. my HSS 1.45mm drill for the M1.6 is breaking every 10 hole, I am running 55 SFM with 0.0009 CPT drilling 6mm deep, with 0.026" peck.

Could one of you guys please give me some guidens.

What SFM should I run HSS drills at in this material?

After how many holes should I change the drill and the form tap?

 

I am already late on this job, so I do not have time to screw around, I will rather changes drill and tap a couple of times extra, than scraping parts.

I know that there aint any written rules, but only opinions and experience, were the last one is what I am lacking.

I would appreciate any help

 

Thanks

Lars

[Lars Christensen]

Gary

Congrats on 500

[JazzBass]

Lars,

 

Use cobalt stub drills and check for runout. With hard materials I try to use the next size up from the recomended drill size. This will prolong the tap life. But you must check and recheck the minor diameter!

[Müřlıń®]

quote:

---

But you must check and recheck the minor diameter!

---

Me thinks you have discovered the secret of tapping

 

On general applications 60% thread is more than enough.........

 

 

will this thread reach 100

[Lars Christensen]

Rick O,

I was thinking on the way home I should have ordrer carbide drills, would cobalt be better in that material?, well I can not get a hold of cobalt or carbide drills before tuesday, and that is to late, so I got to go with my HSS, am I in the right SFM and CPT range?.

quote:

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

But you must check and recheck the minor diameter!

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

So you should have a M00 in you program, so you can check your tap drill size before each tap run?.

 

Murlin,

So you would drill with a ø1.54mm hole in theroy?.

 

Lars

[JazzBass]

If you must use HSS drills, check for runout. After you drill and some holes, check the drill point under magnification. If the drill margins are burning, slow your speed. If they are chipping slow your feed. This works for me, when i'm having trouble with tool life. Take a much closer look at the variables involved.

[Harryman]

quote:

---

the form taps are working great so far (SFM 45 with Hy-Pro Tin coated), but my drilling is giving headaches. my HSS 1.45mm drill for the M1.6 is breaking every 10 hole, I am running 55 SFM with 0.0009 CPT drilling 6mm deep, with 0.026" peck.

---

45 SFM form tapping 316 is WAY faster than I go, but I've been told I go WAY too slow at 6 SFM.

 

On small HSS drills I usally run 30 SFM. They don't last too long, do they?

 

The thing with drill size and form taps is that the distance the workpiece material upsets into the root of the tap is based on the volume of material that the tap displaces.

 

Imagine a cut-away view of a form tap in the hole. Now just focus on one side of the hole. You can see the major diameter points of the tap have pushed into workpiece material, and workpeice material has flowed into the tap toward it's minor diameter.

 

If you examine a formed thread you will see that the material that flows into the tap toward it's minor diameter has a cupped appearance. (This is just the same thing that happens when knurling a lathe part.) As the material flows deeper into the tap, the cupped shape is less obvious and the thread is more pointy, like the minor diameter of the tap.

 

A smaller hole means that the tap must displace more workpiece metal toward the minor diameter of the tap. The minor diameter of the tapped hole becomes smaller and more perfectly shaped. If the drilled hole is too small, the tap tries to upset a greater volume of workpiece material than there is room for, and the tap is doomed to break.

 

If the hole is too large, the tap displaces only a small volume of workpiece material and the cupped shape is very obvious. The thread looks very much like like a double lead thread with one lead only slightly deeper than the other. In this case, the screw having a tapered end, can't tell the difference between the two leads and will sometimes try to start down the minor diameter cup rather than the major diameter point.

 

Since the area of a circle varies with r^2 (A=Pi*r^2)the amount of workpiece metal being displaced also varies with r^2. All this really means is the tolerance on hole size for a form tap is more critical than for a cut tap. Don't guess.

 

Drilling with HSS then form tapping in 304, 316 stainless:

These steels work, (strain) harden. This means that they harden as they flow, or bend. If a dull drill is used, the workpiece metal is not cleanly cut as the drill lip comes along, and it gets pushed around, flowing and hardening in an area very close to the surface on the walls of the hole. Also, the HSS that used to be part of the drill can be getting embedded in the hole walls. Now along comes the lobes on the form tap trying to plow through this hardened mess like a boat bow through rocks on mud...

[ChuckM]

Great advice on the runout and using a larger drill.

 

I'd step up to a #53 drill (.0595) which should put you at 55% thread and you don't need any more for the length of thread engagement you likely need.

 

I would slow the tool down to 30 sfm and use a .0008 IPR starting point. Peck .015 to keep the heat at the tool tip down.

 

Yes, cobalt or better would have been better but if you're strapped for time, you've gotta use what you have. Been there.

Do check with local tool suppliers and see if they have a #53 screw length drill in cobalt. May be an "in stock" item.

 

Never had to drill that small a hole in 316L so I don't envy you. Hope this helps though.

 

-Chuck

[Müřlıń®]

+1 to Harry

 

Work hardening of the tap hole is the other obsticle to overcome.

 

In certain types of steel (p-20, h-13 ect)

drilling the tap hole with carbide will work harden the hole somewhat depending on how friction it is generating.

 

This is why we drill with HSS on these apps.

HSS with 8 to 12 % Cobalt will stay sharp longer, thus using less taps.

 

When the point of your drill wears on the tip sides, it will start drilling a smaller hole and start squeezing on the drill. This will cause friction and work-harden the sides of your hole.

 

Murlin teh take a heliarc and weld a small BB on the tap body and machine tap in a drill press till it breaks

[richardtraver]

if the tapped hole is going to be measured really watch the minor dia. alot of times the thread will not squish enough to keep it in tolerance

[Lars Christensen]

Thanks for taking the time to help me understand the "Magic" of tapping.

I got the SFM for the form tap from OSG, not saying that they are right, just explaining why I am running it at that speed.

I started out with 45 SFM for the HSS drills, and after breaking a couple I lowered it to 35 SFM, but The ø0.106 drill started to have a chatter sound when entering the hole, and it almost looked like the flutes was bending or rolling the edges under magnifying, so I tried to go the other way (45 SFM) and the drill looks better and there isn’t that terrible sound (I am not saying that I am right here, just what I experienced). I am going to try with smaller pecks, I can see how coolant could be a problem.

Any ideas on how many holes a 1.6mm tap can run?

 

Thank you so much for sharing your knowledge, you are true gentlemen.

 

Lars

 

I think I am going to try to make a

[Lars Christensen]

I am going to finish up this job tomorrow, what a pain in the butt, but also a great learning experience. I got some drills in (HSS), and I think they had a bad grind or something, they were breaking left and right, but then I reorder some Chicago Latrobe HSS drills, 30 SFM 0.0009 cpt. .015 peck, and I was back in business. The form tap in the other hand have worked great, I tapped almost 200 holes with that thing, and it just ran like a dream, form taps are defiantly going to be my preference for me in softer material.

 

Again I just want to thank you guy’s for again lending me a helping hand.

 

Thank you

Lars

[Philcott]

Lars,

 

There is another thing to be aware of when form tapping a part with thin walls. Be aware that the process of deforming inside the hole may also deform the outside of the walls. In other words, previously machined walls may buldge out and leave a bump where the tapped hole is. This problem will be a greater issue the thinner the walls are.

 

Phil

[MetalMarvels]

+1 to Phil on the thin-wall parts - been there done that....I usually try to run my tap cycles before I hog out the middles of my boxes now.

[Lars Christensen]

Thats a good tip, thank you Phil.

I have always tapped as the last thing, but maybe this is a good reason not to do that.