Drilling Stainless Steel

[ftownroe]

I am having one helluva of a time drilling some stainless stock. To drill five holes ( #29 size) I have worn out at least half a dozen drills. Are there some special drills that I need to drill this stuff? The holes are only about .850 to .950 deep ( some stopped, some through). I am using Tap Magic and I have used brand new drills and cannot complete a single hole with a drill. I have faced it and bandsawed it w/o problems, but drilling seems almost impossible. I am running the mill drill at 850 RPM. Is this too fast? Any slower just seems to be scraping out the hole instead of drilling and really dosen't get anywhere. This may be a dumb question, but I thought I would ask it before I wasted any more time and drills. I am about to quit and start over with HRS, but I have invested a lot of time in other operations on this piece and still have 13 more holes to drill and tap. I am almost afraid to contemplate the tapping process. Thanks for any help or guidance.

[The Artful Bodger]

I suspect the SS is work hardening.

This is what I would try, but I am not an expert and it may be totally the wrong thing.... get one more drill and a scrap of the material, set the drill press to the slowest speed. Start the drill and bring it down hard on the metal, be brutal. See what happens.

[Westline]

What type of SS is it ....If worked out the sfm correctly you should be able to drill at 2809rpm.
I drilled some 304 SS the other day at 1250rpm with 6mm drill (about a number A drill) and it worked better than I thought.
The number one rule is just KEEP IT COOL...rule 2 is rule one with more coolant
I got irretated with the soluble coolant I have so I just put the air hose right on the tip of the drill and blew like I'm a piggy hungry wolf.
Make sure your bits are at least HSS, cobalt is better but carbon steel is a no go.
Best of luck and stay cool

[Mcgyver]

if I was machining small holes and tapping them in stainless i would want it to be free machining, say 303 or 416. Regular stainless work hardens terribly and if you're not advancing fast enough to constantly be under the work hardened layer created on the previous revolution, you get what you are experiencing.

The local service centres seem to have every shape and size, rectangular, sq, flat, etc of 304 but only a couple of rods of 303 I wouldn't use 304 or a non-free machine type for bar stock unless some property of the job made it absolutely necessary ...weldability for example, which in stainless i never have to do.

[mike os]

welcome to the wonderful world of stainless steel

useful guidance here http://www.bssa.org.uk/topics.php?article=194

those are deep holes for a small bit, why do you need to go so deep?

[Toolguy]

304 Ss

I just finished machining over 300 inches of 3/8 thick 304 plate and drilling and countersinking 15 3/8" holes. I used one 1/4" carbide end mill and 1 each HSS 3/8 drill and countersink. All tools are still sharp and ready to do the next job. The secret to making this work is spindle speed. I ran the end mill at 600 rpm and the drills at 100 rpm with flood coolant. Use a center drill to start on location and a cobalt split point drill. Don't go over 200 RPM, slower is better. Use the same Tap Magic (not the one for Aluminum). Your drills will sink right down and it will be a breeze to tap. The holes you've already started will require a carbide drill to finish and will be very difficult to tap. The holes drilled slowly will tap easily with a good quality sharp HSS tap. If you want to make this work, throw out the feed and speed charts and use sharp tools and run a slow spindle with coolant or cutting oil. You will be amazed at how easy it goes then.

[Mike Burch]

In my experience of drilling stainless (304 and 316) on marine work, slow speed and heaps of pressure, together with good lubrication/cooling, are the answer.
If you let the drill rub instead of cut, the stainless will instantly work harden. You MUST keep the pressure on.

[Boot]

S.S. Drilling

Always use a slow rpm and a heavy feed rate. If at all possible flatten the point of the drill out more than the standard angle. Every thing that is hard to drill: a wider point; every thing soft a sharper point on the drill: like wood and plastic. I drilled and machined Stainless Steel for 37 years and never had a problem . Yes coolant if available or black cutting oil. Air may help cool it ,but it never helped me except to clear chips. We machined every type of S.S. you can think of or purchase. Good luck . Boot

[davidwdyer]

I agree with Boot. (Who probably knows about a thousand times more that I, seeing as how he spent his life doing it.)

Slow speed.

DON"T STOP until you the through or at your stopping point. It you stop, it'll harden and getting started again will be difficult.

[MaxxLagg]

Agree with everything mentioned thus far. I have machined far more SS than I care to remember and it takes a different approach and until you figure out what works, it's pain in the arse.

Slow speed, heavy feed and this:

http://www.nolansupply.com/bysubcategory.asp?category=Fluids+and+Lubes&supercategory=Master+Chemical+Tapping+Fluids&subcategory=Master+Chemical+Tapping+Fluid+-+TRIM%26%23174%3B+Tap+Heavy%26nbsp%3B&type=False&specs=True

This is for tapping but for drilling 304 ss, it is unbeatable. Messy, as it is very viscous but works wonders. One warning though is that it seems to be highly hygroscopic and attracts every bit of moisture in the air. Wipe down all surfaces and tools with some Dykem Remover or alcohol if you get some on it or in the morning you will find a fine layer of surface rust.

[ftownroe]

Drilling Stainless Steel

Thanks for all of the replies. From your responses I guess that I am work hardening the steel by being too conservative with the feed pressure. I know that at some points it seemed to suddenly stop advancing and I was confused until you guys told me about the hardening effect, because it usually started out OK and then became more difficult. I don't have any idea what alloy it is. I would have chosen HRS or CRS, but the place I go to only stocks stainless and aluminum. The hole is that deep because that is the cross sectional dimension of the material. The holes are to be counterbored for half an inch, so for the future holes I may drill the larger diameter first, then finish the bottom of the hole with the smaller drill. I will also try to find some spray lubricant which will aid in the cooling process. Thanks again, I will let you know how it goes.

[macona]

At that depth you want a parabolic bit. But thats even deep for a parabolic. They are good to about 12x diameter.