Drilling big holes in 304 stainless steel

[alan wParticipant @alanw]

I want a 20mm diameter blind hole which is 40mm deep down the centre of some 304 grade stainless steel 35mm bar.

 

I'm using a lathe and I bought a set of "blacksmiths" drills at 15, 17.5, 19 and 20mm. These have a 13mm shank which fits a standard tailstock drill chuck.

 

I find the larger drills have been blunted at the outside corners of the cutting edges. Re-grinding them is no good -they blunt again instantly.

 

So I went to a boring bar with a rhombus-shaped new insert. Fully tightened in place. The finish is dreadful – heavily ridged – no matter how fast the piece spins (1500rmp) or how light a cut or how many times I run it up and down to do "spring cuts". Plenty of cutting fluid.

 

I'd be grateful for any useful insights or ideas you may have.

 

Is there any point in buying more drills with cobalt coating? Titanium?

Would 303 stainless be significantly easier to drill?

 

Thanks

[alan wParticipant @alanw]

it’s not going well and I’m out of ideas

[VersabossParticipant @versaboss]

1500 rpm, dia. 20 mm in stainless??? That's about 10 times too fast, imho. No wonder your drills get blunt!

Blacksmith's drills are maybe not the highest quality, but a substantial boring bar (12 mm) should have no problem, especially if you use a sharp (so-called 'Aluminium&#39 insert.. Or even a good, sharp HSS boring bar…

Regards, HansR.

[Martin KyteParticipant @martinkyte99762]

cut don't rub.

[Ian S CParticipant @iansc]

Use back gear, and use a fair amount of pressure to keep it cutting. Some Blacksmith drills are carbon steel, if these get hot, you'v stuffed it, best use HSS. Start with 8 mm /10 mm, then 1/2" 12 mm, then use the drills you mentioned. One of the first things I made when I got my lathe was a hot cap for my first hot air engine, 1" bore, 2 1/2" long, with a 32 tpi internal thread in the open end, in a piece of 316 stainless, it just takes time.

Ian S C

[Ady1Participant @ady1]

Slow speed with backgear, use sharpened fancy hss, M42 etc because most carbide chips under high pressure

(non-chipping carbide may be available)

Slow speed, high torque, sharp tooling and a nice stiff lathe, no sloppy bits allowed

Edited By Ady1 on 19/10/2015 14:31:13

[duncan webster 1Participant @duncanwebster1]

If you only take a little bit with a drill it is only cutting right on the corners and so will blunt very quickly. If the lathe will take it go for 15mm then 19m and bore the last bit to get a finish, HSS for preference. Keep it cutting or the stainless work hardens.

[John HaineParticipant @johnhaine32865]

Has it work hardened?

[John Stevenson 1Participant @johnstevenson1]

304 work hardens just looking at it.

Bin it, buy some 303 and you will never look back

[Steve PaveyParticipant @stevepavey65865]

I was never taught to drill a series of gradually bigger holes, just a centre drill (or spotting drill if you have one), then a pilot drill just a bit bigger than the web of the final drill, followed by the final drill itself. Going up a couple of mm at a time is guaranteed to knock your drills to hell.

Slow, plenty of pressure and some cutting oil, and make sure all the cutting edge is doing the work. Once it work hardens you're stuffed.

[Anonymous]

Got to agree with the last two posts, I'd never move up a mm or two drilling 304, if it's a large hole then it's one 13mm drilled hole then a boring bar with plenty of coolant, but as JS says it's 303 every time you can as it cuts lovely and doesn't really heat/work harden.

[Ian S CParticipant @iansc]

Alan doesn't say which lathe he is using, if he has a reasonably large lathe, with a good amount of HP, drill a pilot hole just over the thickness of the web of the final drill, then straight in full size. But if he has a small lathe, Myford or smaller, he might not be able to get the larger size drills to work, so boring might be the way to go.

I think this was made from 304 stainless, the bloke at the ware house where I got the steel from reckoned I'd be pushing my luck  but as it was the only bit of stainless in the scrap bin he gave it to me to have a go at.  It has a bore of 30 mm, and a 32 tpi thead in the open end.

Ian S C

Edited By Ian S C on 21/10/2015 11:10:08

[alan wParticipant @alanw]

Thanks for all the replies folks – much appreciated.

 

Versaboss: The 1500 was only for the finishing "spring" cuts when all else failed to remove the ridges.

It was a 2mm boring bar that gave me the ridges. New insert. Lots of lube.

But I don't recall the normal cutting speed I used – so one way forward is to try again at about 150rpm. Thanks.

 

Martin. Yeah. Thanks.

 

Ian: OK I googled "back gear". I don't have one.

However, I think getting them hot was a problem.

I did go up through the drills as you mentioned, though some of the Youtube boys don't and it seems to work fine for them.

On the last hole like this I drilled the 20mm drill's shank was binding in the hole near the chuck. I reduced it with emery but I still had to fudge a worrying bar arrangement to stop the tailstock spinning. It got the job done but it wasn't a happy experience.

So – maybe buy some more Blacksmiths drills and watch the temperature closely and much slower speed.

 

Ady1. OK. Look for HSS M42.

 

John Haine: Maybe – I researched that, but I don't knwo how to tell nor how to avoid it.

 

John S: Use 303 – Oh – bummer though – I got quite a bit of it.

 

Steve P: Hah! I wondered about that. So go big and slow.

 

Mick B: Another vote for 303. Bugger. Thing about a boring bar is it's really boring! All that measuring and – well – engineering stuff. I just want the damned hole. Bam.

I'm stamping now and I'm going to sulk.

 

Ian S: It's a small Chinese lathe.

 

OK, so I'll but ONE new 20mm blacksmiths drill and try drilling in one go – slow – after a small pilot.

If that fails I'll try 303.

 

Thanks very much for all your help.

[Ian S CParticipant @iansc]

I thought it might be(small Chinese). Get a good quality HSS drill, it might cost a bit now, but you'll have it for years.

All my bigger drills, there is not too many, are second hand, and some are getting worn on the out side of the flukes, which means they tend to jamb up if I'm not careful, that's why I say get good ones.

Ian S C

[Martin ConnellyParticipant @martinconnelly55370]

Where I work we drill a lot of holes in austenitic stainless steel pipes. All of the larger drills were blunted at the corners and produced nasty rags on the inside of the pipe. When I investigated what the problem was it turned out that almost all of the pipe fitters had been told to reduce the feed per rev (using a large radial drill) when using larger drills. This is completely the opposite of what you should do. If you think of the cutting edge of a drill as a chisel then it should be obvious that there is a suitable angle to drive it in at. Too steep and there will be too much force required, too shallow and the chisel will skate along the surface. If you consider the right angled triangle formed by the circumference of the drill and the feed per rev it should be clear that in order to maintain the resulting angle the feed needs to increase with increasing diameter. The damage to the drills and the rags on the inside of the pipe was caused by the drill pushing rather than cutting its way through the pipe wall. Correcting the feed per rev improved the life of the cutting edges and the time taken to deburr the holes. A suitable feed and speed chart stuck on the drill fixed the problem.

The feed per rev for austenitic stainless at 20mm should be about 0.21mm. If we apply this to your 20mm hole and a speed of 100 rpm on the lathe then we should be feeding the drill in at 0.21×100 = 21mm per minute. At 300rpm you would be going at 63mm per minute.

We then get to the question of to go up in steps or not. If you need to feed at 0.21mm per rev for 20mm what is this doing to the inner edge of the drill with say an effective diameter of 10mm. Well at 10mm the recommended drive is half that at 20mm so the feed is far too high for the inner part of the drill. Trying to push the drill through the stainless with a small pilot hole will probably result in a feed that is too slow for the outer edge. Small pilot holes and then drill to size may work with more forgiving materials than stainless.

In summary you should use the correct feed and speed for drilling holes and step up probably a maximum of 4mm at a time to ensure the cutting edge of the drill is doing its work as it is designed to work. Recommended maximum speed for 20mm diameter and austenitic stainless is about 350 rpm

It is also important with work hardening materials such as austenitic stainless that the tool never rubs as it will cause work hardening which will take some effort to get through without resorting to carbide cutting tools. Keep the pressure on or back off quickly to avoid rubbing.

If you get an ER32 chuck to fit your tailstock you can put milling cutters with shanks up to 20mm in it. If you get a three flute centre cutting end mill you can clean up the hole to its final size and get a flat bottom to the hole. I would probably drill out or end mill to 16mm before the final pass. Additionally the three flutes are stiffer than a twist drill and will give a better result than a twist drill.

Information on drilling feeds and speeds is readily available, search for drilling speeds and feeds chart images on the internet.

[Author]

Posts