Trouble Tapping Stainless Steel

I assume you changed the size of the hole when you changed to a roll tap?

Plenty of oil on the tap?

Yes there is plenty of oil getting sprayed on the taps and the hole is changed to the correct dia. for the roll tap. one thing I forgot to mention is the steel is 304 stainless with 9% nickel .185 thick 5/16-18 tap.

I forgot to ask, how many holes per pc.? If it's one, yea, I'll try to help you, it it's 20 holes per pc. well, 600 holes is not to shabby for a roll tap.

Type of lead on the tap, is it a plug or hand tap lead. (how many turns before your first full thread?)

It is a Balax 4 groove bx super tin coated plug tap and it is 1 turn to the first full thread. There is one hole per part. I know that I will have to replace the taps after a while but I have to run 50,000 pcs, a month.

Its the nickel content that is the factor here. Try another form of lube, reduce the cutting speed. Try a copper based lube? Do you use a taper tap before the plug. Are you going into a blind hole? How deep is the hole? Can you heat the hole before tapping? Do you have the hole sized correctly? Just asking.

304 stainless readily workhardens. 304 doesn't harden by thermal treatment, only by cold working. Any tool dwell will create a harder less deformable zone or 'skin' which the subsequent tool needs to get thru to be effective. If you elect to anneal don't forget to re-passivate. Not sure that roll tapping this grade would be my preference.

milo

I would like to use a cut tap but the die is not made to dispense the chips created by the taps and I cannot deviate from the specs. of the customers part print, so this is the matl. I have to use.

use an annealable alloy that can be hardened after the final tapping.

First anneal after the extrusion

Then the tapping and last the hardning (at least when you want the hardness)

the rolling will result in a hard surface on the thread, but I assume that you want this zone to be softer and another surface to be hard.

What alloy are you working with?

This part is running in a progressive 2 out die, there is no room or time for what you mentioned, it runs at 40spm.

Consider reducing your thread engagement.Very little strength is lost by a reduction to 70%. Also as your material is already work hardened and further work hardened after roll tapping the overall strength of the threaded hole will be higher than the surrounding metal. This should take some of the wear and tear off your tap.

Then experiment with different tapping oils, Molybdenum is a good one for stainless steels

I'am going to try the 70% thread with an OSG tap that is made for this application, I hope it works, the taps are $32.00 each. then I will look into the lube.

thanks

The tapping of high tensile and normal stainless steels should never, in normal circumtances, be attempted with a drilled hole giving practically a full 100% thread. This considerably overloads the tap and will almost certainly lead to trouble with material of this type. A drill size giving a maximum of 75% full thread should be used; for long holes 65%/70% is quite sufficient and should not be exceeded where small sizes are concerned.

The importance of keeping taps sharp is a must but it should be remembered that for austenitic stainless steels it is equally important to keep the tapping drills sharp as well.

Dull drills with rounded corners and worn lands may leave a work-hardened surface inside the hole to be removed by the tap. the extra load thus imposed is likely to prove too much for an already highly stressed tap and may be an unsuspected cause of breakage.

hope this can be of some help to your problem.

I had the same problem many years ago with an external rolled th´d! turned out that the tool cutting the primal diameter produced a work hardened surface which greatly reduced the tool life of the roll die. If the process is a second op, then it is of great importance to ensure minimal work hardening of the first op! Refer to the mat.spec for cutting speeds and feeds. Turned out that the only way to combat the problem was to start with a slow spindle speed and high feed for roughing and with a dedicated finishing tool, turn the diameter to 70% effective thus removing the work hardened surface. With roll tapping we found the most important factor was the coolant and the thread lead angle. The coolant we used was a tryc and light machining oil mix. Don´t know if you can still get tryc, It was a very thin cleaning agent about 15 years ago! Hope I have been of a little help!

Some good suggestions from you all, who clearly know far more about it than I do.

However, my Stainless worker says that if he can hear the drill bit (juddering), it is time to resharpen the drill bit as other wise the SS work hardens and the rate of work falls rapidly.

As has been said, the drill runs at a very very low speed, but the feed rate is higher to cut away the metal rather than work harden it.

If there is any squeaking or the slightest blue colour to the swarf then the drill bit is blunt, also use a soluble oil water mix for the lube (Suds) and keep the feed rate low so as minimize the contact pressure so the drill is just cutting if the swarf is chipping then your feed rate is too high. You will never get a perfect curl but at least make sure the swarf is shiny. Set the clutch on your tapping machine so that the wear on the tap disengages the drive when the work piece may start to harden. Parafin makes a good tapping lube for SS 304. Just don't smoke or let the tap get too hot. The rest has all been said.

Too light a feed, on the drill, will surely result in workhardening of area to be deformed by the roll form tap. Blue color on a chip indicates heat is in chip and not in tool, I agree that to start out I would reduce Speed (which is that which causes heat - as opposed to feed) in this grade of stainless.

milo

As another sugested make sure you are drilling for a lower percentage of full thread such as 65%. If you are drilling in a milling machine which has more rigidity than a drill press you can get away with using carbide drills at a higher rpm. This will lower the work hardening problems and speed up production. Balax and OSG are two of the best taps available. You may want to try tialn coating as opposed to tin. One of the most important issues is your cutting oil even though you are not actually cutting with the tap. Moly-D is about the best. There are a few others that are very sticky that are especially desiged for tapping dificult materials.

Lots of problems threading a 304 SS 1.25" deep through bore for 3/8 x 24 screw. Is it economically possible considering the time to do the job, short run on tools, ruined pieces, etc.?
The product if successful will need monthly production runs of several thousands, and requires two threaded bores per piece. Aren't brass inserts easier? Been told it's almost an art to press-fit inserts into SS, and therefore hardly practical for mass production. Would appreciate some answers as to the best way to put threads in the bore. Thanks very much. Mike

Unless you have some reason for 1.25' of thread you should reduce the depth of thread to 5/8" this much engagement is stronger than the 3/8" bolt and will be much easier to tap.