Tapping 304 stainless

[Vern Smith]

I have to drill and tap about 300 1/4 - 20 through holes .5 deep in 304L stainless. The "L" is for improved weld-ability they tell me. I would like some ideas on speeds and feeds for the drilling and suggestions for the tapping.

My research says 500 rpm and 4 IPM for the drill. Would you make one peck or go all the way through? I know work hardening is a big issue with stainless.

I was planning on using a form tap, Balax coated, both with flood coolant 10 to 12% oil. A side issue is whether to go all the way or peck tap.

Thanks in advance for any suggestions.

Vern

[Donkey Hotey]

I think the 'L' is for low carbon. The good news is that it's supposed to be a very machinable alternative to the standard grade of 304--or so I've been told. That's all I know but I'm very interested to hear the rest of the advice.

[Vern Smith]

I doubt if we will have to wait long. That's what I love about this forum.

[dertsap]

Vern i think youve already come to the right solution , run it
if there was anything else to suggest i would go for cobalt drills or better yet solid carb

[mc-motorsports]

Carbide is best, but you have to run a good coolant flood, if the drill hits a chip before it's engaged and cutting, it will chip the drill, same for cobalt but not as bad. I think your feedrate is a little aggressive, use screw machine drills for sure. They sell special taps for SS and titanium, I suggest you invest in them, a HSS tap would be lucky to make it through one hole. You'll just have to break a couple of tools and fine tune your parameters, blah!

HAVE FUN! I HATE SS!

And yes, "L" stands for low carbon. During welding, carbon tends to react with the chromium content and form "cromium carbide precipitation" or "that funny looking black crap" on the back side of your weld if you don't back-purge or heat-sink it. 304L has almost no carbon content to help avoid this.

Good luck!

[shay z]

use cobalt drills. they are the best solution fir that kind of job.

if you can buy western european materials (but not fro spain) ut will be easier for tapping.

I use french materials for machinning and i save on tips, taps and drills much more than the cost difference between chinese or indian material.

drill the hole in one pass. it is not deep.

I use hanita or titex taps and making approx 700 threads per tap (1/4 NC 20 m"m deep blind hole) with tapmatic gold cutting oil.

[Vern Smith]

I appreciate the replies, I use cobalt short drills as a matter or course so that will fit nicely. Any thoughts on the peck rigid tapping?

Vern

[PBMW]

I would not peck tap it. Stick it through. I would run that HSS tap at about 40 or 50 sfm. I would use a carbide drill if you were in a hurry. (Who isn't) but you need to have someone there to catch it if something goes wrong. Otherwise, cobalt. Talk to Gurring, or Titex. Another thing I like to use is MA Ford Hi Roc drills. They are awesome!!!
I do 1/4-20 holes in 316ss all the time at 200 sfm with Hi Roc drills. No peck. Feed about .0045 per rev. It might be a little disconcerting at first...

[slatern44]

Vern. If it was me I would get a #1 carbide drill, coated balax tap and go for it. One shot on the drill and the tap. You should be able to get it done on one drill and tap. But if you have a cobalt drill you may have to change it once or twice to get the job done. Have fun!!!

[gizmo_454]

Ah yes. Stainless. Everybody loves it...Can't you tell? We run quite a bit of stainless. On any kind of a through hole like that, I would recommend a spiral point plug tap. They cut freely and push the chips out the bottom, so they won't clog the flutes. We normally use OSG ExoTap for tapping stainless. We have tried others, but they seem to hold up better for us.

As for the drilling scenario... It all depends on the equipment you are using and what you want to spend on the tooling. If you are using through tool coolant, I would recommend Mitsubishi's MWS drills. They are a bit pricey, but again, they work wonders. As PBMW said above, it is a little disconcerting at first. One job I run one on is a 0.318" diameter drill. Running at 2500 RPM and 0.006" per rev feed and the hole is 1.175" deep, in one pass. No peck. If you don't want to spend the money on Carbide, I have used OSG's EX-SUS-Gold HSS/Cobalt/TIN coated drills with good success. Again, no pecking.

There are a number of ways to do the job at hand. Some faster than others. It's just a matter of what the job warrants when it comes to buying the tools. Obviously, you wouldn't want to spend $150 for a HP Carbide drill for a $100 job. In the end, it all comes down to what works for you. Good luck, and have fun!

Gizmo

[HuFlungDung]

Surprise me and tell me that the form tap worked good when you're all done I'd be too chicken to try it. By definition, a forming tap is workhardening the material, and the nickel in stainless has a great affinity for welding itself to whatever it is rubbing on it. Cut thread tapping isn't so bad, just keep an eye on the tap for even the slightest bit of damage will cause grief. I always use a sulfur bearing thread cutting oil.

[dertsap]

Originally Posted by HuFlungDung Surprise me and tell me that the form tap worked good when you're all done .

i never beleaved it till i tryed it , i ran production runs of 304 3/4" round stock that had flats milled on the side then drilled and tapped thru , it never took to long before the tap would fatigue and eventually break ,i nearly had it down to how many parts i can do then change the tap before it let go ,
then i had a guy suggest trying form taps , though i thought he was nuts i figured i had nothing to loose but a tap and another part , sure enough it worked great ,
i always went to the max allowable drill size which helped some , even at that the thread was stronger than any bolt thread