O/T- Threads!!!!!!!!

[RStuart]

Having some trouble tapping 300 series stainless again. The problem seems to come and go with material lots. Trying to tap 3/4"-10 thru an 1-1/8" plate. Tap keeps over loading the machine. I would like to go to a lesser thread engagement but our train operators give me the whole roasted pork bit."We've done it like this foever." Was wondering if anyone could guide me in finding some information as to determining a pressure rating vs. thread engagement. Some sort of engineering calculation. Like, for instance, a 3/4"-10 thread at 75% engagement, 1-1/8" deep is rated for 200 psi. Or whatever. Something like that. Our engineers earned their title because they can draw stuff. I am a little bitter about that if you can't tell. Any guidance would be greatly appreciated.

[crazy^millman]

Thread mill that bad boy is what I say. Unless you got 50 taper you will have trouble unless you peck tap at .025 step downs and I can hand tap faster than that. Tell your opetors to grow soem balls and tap them by hand or if you have a radial drill press get a morse tap holder and power tap them on there us to do 1-1/4 7 thread in 304 SS all day long 2" deep on our radial drill press back in Florida.

[mayday]

drop back to 60-65% thread. or

Millmans idea - radial drill, frees up the CNC for more impotant stuff

[RStuart]

Unfortunately I am the programmer, set-up guy and the operator!!!

[RStuart]

Would like to go to 60-60% but I am getting flack that it may not hold the pressure and I am looking for something to prove either way.

[Guest CNC Apps Guy 1]

3/4-10 Max. minor dia is .663 Get as close as you can to that, use an e/m after drilling if you need to. Peck tap (better) or thread mill (best) as was stated earlier. The closer you get to the max minor dia. the less cutting pressure you'll encounter, though SS it tough stuff for the most part any way. Kick those buzzards to the curb and get some new blood in there.

[Jack Mitchell]

RStuart,

 

Machine model and size would go a long way with helping with your problem.

Please use an interrupted tap with some sort of sulfur chlorine based tapping oil.

 

Over drilling the tap drill will definitely help if you can get away with 60% as opposed to 75%.

 

If stalling then try bumping up the rpm by another 20% - sometimes this will work.

Personally, my VQC15-40 Mazak would probably stall out as well.

 

Good luck – give the operator a very large tapping handle and put his strength to use if all else fails. (Feeling lazy? Then send the guy home)

 

Good luck

 

Regards, Jack

[Guest CNC Apps Guy 1]

Do you have certs for the material? Make sure that the hardness, nickel content, carbon content is within spec. Seems like if you're getting that much variation in toughness/machinability there could be a problem.

[Jack Mitchell]

Sorry, it would appear that there have been a lot of responses between reading this and posting back. (Prhaps my typing skills are a little bit slower)

 

 

Regards, Jack

[Fig sign]

I grew me the balls as Millman said and threadmilling and handthreading anithing more then M12-M14 .

Also very important the taper geometry ,look through manifacture cathalogs ,there are some goood tools .

Tool geometry is important for the load ,for example a taper for taping

through-out threads (strait one ) differs a lot from helical taper with a little leading cone .

[Rekd™]

I'm fairly certain a 60% or even less thread on 300 series with a 3/4" tap well over a full diameter deep will hold as good or better than the bolt they're gonna put into that hole.

 

'Rekd

[crazy^millman]

Well when you are making stuff for Power plnats and Paper mills they want it right and the 72% amount. I done my share of Stainless over the years and Thread milling is easy fast and very effective. I got stuck with soem welders hard facing some pump housing for the company I was at that went into a Power Plant. They were $600,000 a piece and we had 12 of these housign they wleded up wihtout thinking of not welding into the thread area. I had been there about 2 weeks and the hot shot know it all guy they had keep tryign to tap a 7/8-9 helicoil in a VTC-20 Mazak. No way no how dont care if you put a 20' cheater on the spindle was not going to do it. I told them to thread mill it. They all laughed the owner the enginner fro mthe power plant and about 3 others. I put a years salary up that I could do and it could be done in minutes verse the 3 weeks that already had to this point trying it there way. Noone would put up the money but I went and borrowed the tool and holder I needed from a place I use to work. I wrote the code long form doing a 3 sub tier and hit the green button did 18 holes in about 35 minuts and they where within .002 of the needed P.D. Do what you want but time is money and money and money is time and I just type person do to it and get it done the best way and quickest way possible if that means a little sweat then tell to tuff it up. I am missing a splien, have a lung that is part collasped, I have a bad shoulder from a car accident and promise you I can tap 50 of them holes a day by hand if I had to.

[Fig sign]

Bravo ,Millman ,noone would say better !

[Code_Breaker]

quote:

---

Thread milling is easy fast and very effective

---

+1000 for Millman

 

This is the only way to tap stainless steel.

 

Code_Breaker

[mike_f]

I would agree, thread mill. Keep in mind that 304 will work harden from the drill, the chamfer from your spot or center drill can also become work hardened wearing out the lead on the tap almost immediately as it enters the hole. If I had to no choice I would be talking to Emuge for taps, pricey but effective.

[RStuart]

Doing this on an Integrex 400IIY. Also, I am the operator, programmer, set-up as I stated earlier and I sure do not want to tap by hand. I am milling the hole to the max diameter gor 75% engagement but still only can tap at about 25-35 rpm. Working with 316L SA240 and the certs are in spec. Looked into thread milling before and could not find an indexable tool that would work. Carbide thread mills a little pricey for management compared to taps. Currently with the stocking jobs that we have on the floor I will be tapping 570 3/4"-10 holes. And this occurs roughly about every six weeks. Still looking for hard proof that I can reduce the engagement with out reducing the strength.

[RStuart]

Also another one of my reasons for wanting to decrease the engagement is due to when the units are finally assembled in house we sometimes have a problem with thread gulling and the all thread getting stuck in the hole which in turn we have to cut out by manual methods due to the fact that the unit is now so large we have no machine to put it in. We are using monel all thread due to threading stainless into stainless is prone to gull. This has been a reaccuring problem since before I worked here. I am just trying to get rid of it. Still looking for hard proof that I can reduce the engagement with out reducing the strength.

[McRae]

One other thing that may be influencing the thread is the tap itself. Use a spiral point tap to push the chips in a thru hole. If you are using a conventional hand tap, the chip gullets will fill up with swarf and you will overtorque because of this. Also use plenty of thick threading paste applied to the hole - not the tap.

 

My favorite tap is an emuge and this will work very well for you.

[RStuart]

We use emuge taps they work pretty well when I can get the darn thing to go through. We are using a spiral tipped, coated tap.Still looking for hard proof that I can reduce the engagement with out reducing the strength.

[Harryman]

See if you can find a Mark's Handbook for Mechanical Engineers. I'll bet it would cover the subject.

[C JAYNES]

RStuart,

Try this site they have a demo version of a calculator to figure your thread engagment question.

http://www.boltscience.com/pages/strength.htm

[HEAVY METAL]

General rule is thread heights over 60% of thread do not increase the strength of a threaded joint and it is an advantage to favor the use of larger drills. In s.s 50-55 % and still be safe.

[McRae]

This was very informative - this section in particular.

 

<

 

The effect of a low proportion of thread height is to reduce the shear area of the external thread, this is illustrated in figure 1. For very low thread heights, the shear plane through the threads need not be parallel to the thread axis, this is illustrated in figure 2. Such failure modes are difficult to predict and can be easily eliminated by maintaining a reasonable percentage thread height.>>

 

In general - 1.5 to 2 times thread engagement at 60% will be sufficient. Thread Quality and acceptance is defined by ASME and the pitch diameter is the principle concern. See Machinery's for more information.