Tapping 0-80 in 17-4PH

[metalhead88]

I need to tap 0-80 holes in 40 17-4PH rings.
Each ring has 8 holes. It's a thru hole 1/4
deep.The mat. is not yet heat treated.
Drilling wasn't a problem. I've tried several
taps the best one being an EMUGE tap. I tapped 18 holes before it failed. At more
than $40 a pop it's an expense I cannot
afford. Greenfield was next best but I can't
find a dist.Any help would be appreciated.
Fred

 

[TVP]

Stainless steels exhibit a number of features (high toughness, high work hardening rate, etc.) which lead to difficulty when performing any machining operation. When tapping, the following recommendations are helpful:

1. Use taps that are as large as possible in diameter (high side of the tolerance.

2. Keep the percentage of full thread as low as possible-- 60 to 75% is a preferred range, but where the depth of the tapped hole exceeds twice the diameter of the tap, it is economical to use only 50% thread.

3. Use a flood of lubricant specific for stainless steels. Mixtures of sulfurized oils and paraffin-based oils may be best. Use two streams of cutting fluid, one for each side of the tap, during the entire tapping operation.

One source of problems during tapping is the work-hardened surface that was produced during the drilling operation. If you did not optimize the drilling parameters, you likely produced a highly work hardened surface. And regarding the tap itself, you only mention brand names. What type of geometry did you pick? From what material is the tap made? Stainless steels require specific tap geometries, and the tool material should probably be a nitrided tool steel like M7 or M10.

 

[jbel]

Wow!!!!! 18 holes with one 0-80 tap in stainless steel!!!!
You should be on your knees praising Emudge for making a tap that good. We use Emudge taps exclusively because of the high quality. I would be thrilled to get 18 holes from one 0-80 tap in stainless steel.

Here's a question for you...

What is more expensive, buying a new tap every 15-20 holes at $40 a pop or struggling to get the job done and ending up with at least a half dozen broken taps that need to be EDM'ed out at the end of the job?

Me thinks the Emudge taps are not cheap but they are inexpensive compared to trying to remove a handful of low quality broken taps.

 

[BobUXL]

As TVP was pointing out, use a good high performance tap. One where the tap creasts are tapered to reduce rubbing. Secondly, look at taps with straight flutes. Do not get a tap with an high helix. These taps tend to spread and jam in the threaded hole during extraction.
As far as materials, also look at M2 taps. This material has a higher toughness than M7 & M10. Use a TiN or TiCN coating. The coatings will increase lubricity of the tap. The TiCN coating will increase wear resistance. Stay away from a TiAlN coating. Yoiu are not generating enough heat to take advantage of the coating.

As also said, use a good petroleum based lub with plenty of sulfur compounds and high pressure additives. Many lubes for tapping have high concentrations of these additives.

Plus, for the next round, you may want to consider the material source. Get a high quality, enhanced machining alloy like Ugima 630 from Ugine. Many distributor 17-4 alloys are not necessarily balanced for good machinability. Yes, the enhanced versions cost a little more, but the machining performance makes up for the increase price.

 

[unclesyd]

We used 17/4 for quite a few components that required a lot of fine machining. We always worked the material in the heat treated condition, H1100. The best lubricant we found was made by Tap Magic. The material also worked very well after the double H1150 heat treatment.
There original formulation of Tap Magic had trichloroethylene as component and was the best. But even after the removal of the trichloroethylene their products continued to perform. We also used a very heavy cutting oil, as used in pipe threading, on the very small holes. It was interesting that we could go from a very thin solution of triclean and oil to the very viscous sulfurized oil with essentially the same results.
Just for information:
Also water will work very well. Deodorized kerosene, Deodorized kerosene + lard.
On very small holes, don’t laugh, spit. The technicians would use it when they had only a few holes(0.0015" -0.0030&quot to drill.

This is a link to MSC and Greenfield Taps, I hope

http://www.mscdirect.com/IWCatSecti...d&NameVector.length=2&View.x.x=83&View.x.y=12

 

[sc0TTl]

Hi metalhead.

From my experience, you should get more holes than 18 per tap in 17-4Ph SS. Things to consider:

-use a straight flute, spiral point tap to help eject the chip through the hole. Make sure that the tap is fed far enough to get past the 3-5 threads of chamfer at the beginning of the tap. If you do not do this, then the chip will not release and upon reversal the tap will try and recut the chip and snap.
-using a tap fluid with high sulfur content is a good recommendation.
-when drilling, take the minor diameter of the thread as big as is acceptable.
-make sure that when you drill that you do not build up to much heat and work harden the material because this will make it difficult to tap. 17-4 work hardens fairly easily.
- try a tap with a powdered metal substrate. These taps do a nice job of filling the gap between HSS and carbide. They are both wear resistant and tough.
-TiCN is a great coating for taps. To really optimize it, have the tap coated with both TiCN and a soft coating like Guhring's molyglide for extra lubricity.


good luck.

 

[EdDanzer]

You might try 2 stroke motor oil as a lubricant. We experimented drilling 500 BNH plate with TiN coated HS steel drills and found this to give the longest tool life.
I agree with TVP on using a larger drill size to reduce torque.
The best option is to reduce the tapped length to 3d, .180 deep or less. Most nuts are thinner than the diameter of the thread. The customer may be able to use longer screws so the hole can be larger at the top if the thread depth cannot be reduced on the back.