Trouble Drilling 316 Stainless, God save the drills they're dying all around me

Hey there guys,

I'm a first time poster here, I always look at the forums for tips and tricks and figured it was time for me to register.

I'm trying to get through a 14.75 x 14.75 1 in. Thick plate of 316L stainless. I'm tooling on it in a VF-6 HAAS vertical Mill, with the New Gen controller, with BobCAD as my CADCAM software. I'm 25, and didn't know what machining was a year ago, and I'm now fabricating for a prototype R+D Shop as one of the only 2 CNC operators/programmers. What little training I have was Manual Machine based, so losing the tactile feel and squeal of cutters on the material has been difficult for me. not to bore you with my whole life story but just to give context as to what my background is. I'm over my head every day of the week.

This plate has 16 perimeter holes thru, at .391 diameter. then a .27, .16, and a .44 for good measure. I'm trying to pilot drill these diameters with a .140 HSS Twist Drill from when Jesus was a private, but I'm snapping these little f***ers like a Husky in a pile of pigeon bones. My supervisor has approved that I can order tooling if I need it, but he wants me to make sure my speeds and feeds aren't whats blowing my bits.

I've done as much research as I could into Machinery's Handbook, youtube videos, and any forum I can find related to speeds and feeds for stainless steel but I'm still burning bits. I've only run the .140 Bit so far but these are the speeds I came up with;

.44 Drill
RPM= 260.5
Feed IPM= 1.0

.391 Drill
RPM= 293.1
Feed IPM= 1.2

.27 Drill
RPM= 424.4
Feed IPM= 1.7

.21 Drill
RPM= 545.7
Feed IPM= 2.2

.16 Drill
RPM= 716
Feed IPM= 2.9

.14 Drill
RPM= 818.6
Feed IPM= 3.3

To reiterate, I've only attempted to Pilot drill with the .14 so far, and haven't made it through that operation yet. I realize this stuff work hardens quickly, but on my last two breaks it was near the middle of the plate or at the end. I'm Peck drilling at .020 a peck.

I appreciate any input provided, and am definitely interested in tool recommendations or personal experiences. Thank you very much!

Whats your coolant concentration like? Stainless is a bit like aluminium and likes its cutting lube to be slippery!

What drill bits are you actually using too? HSS alone is a pretty broad term!

30 sfm = 818.6 rpm, this is reasonable
.02% x .14= chip load, IPR=2.3
I think your feed is to high.
I would peck .5D to 1D, with flood coolant.
I would spot drill 1st, then peck drill all holes.
If I understand your post, you are doing a pilot hole 1st & then opening up each hole.
You should be able to drill to size with an onsize drill, for each hole.
Step drilling might workharden the holes and make life difficult.

I'd be using cobalt stub/screw machine drills(split point), I mostly use PTD, and usually no pilot for that size, 25-30sfm, lots of rich enough coolant. There's fancier drills if you want to throw $ at it and the qty justifies it, but this serves me well for the cost and my needs. I find pecking every 1/4 to 1/3 dia usually works ok in stainless for around those drill sizes. I always tend to be on the cautious side when I drill cnc, manual I'll go with feel and push harder in most cases...

We stay around 45-50 sfm usually. But slower never hurts in SS. Speed burns, feed breaks. Cobalt 135* is our choice and no step drilling. You def could lighten that feed up on small drill.

I would either go to Guhring's website or contact a Guhring Application Engineer.
530 Series Powdered Metal with Firex should work well.
http://www.guhring.com/Products Services/Tools/?Type=24
Speeds and Feeds on same page.
Not going to be HSS price but you should make it up in productivity.

Could drop back a little to 657 Series
Cobalt with TIN
Guhring, Inc. - Tool List

+1 on powdered metal

The small drills I'd run up around 2.5k rpm, 1-1.5 imp, peck every 20k, the .21 and .27 around 1800 rpm, 2 ipm, peck even .50k, the .391 around 1500 rpm, 3 ipm, peck every 100k

It's 316 stainless, not tool steel...it's gummy so you gotta clear the chips, but it likes to be driven not tinkered with. Flood the piss out of it with good coolant, use a refractometer if you have one, and keep it on the more concentrated side. Get some good TiAlN coated hsco drills...not expensive and will punch through much easier.

There are some nuances that may be missing here but important. Great advice given from others so far as well.

When you're pecking, it will help not to rapid down to the bottom of the hole. You want a bit of clearance approaching the bottom of the hole (say, 0.030" or so) so that if there's still a chip in there you don't pinch it between the bottom of the hole and the drill. That's a real quick way to "pop" a drill bit. With some clearance, it's more likely to slide into a flute and be clear of the cutting edge. For the larger drills, and in terms of chip evacuation, you aren't really into pecking depth, but it doesn't hurt anything if this is making it easier for you. It is probably more important for the coolant though. Keeping a drill "down hole" too long can starve it of coolant and heat builds quickly.

Unless there's some kind of rush or lots of parts to get done, back off your feed by maybe 25-50% and small pecks (0.030" - 0.080") with lots of coolant and/or air from the SIDE (not the top) to clear the chips and not force them back into the hole (though this may not be necessary if the chips are small and being pulled out of the hole by the drill already).

Forget the pilot drilling, but definitely spot the holes if the location is important and/or you aren't using stub length. Use split point for reduced drilling pressure, but this is more of an issue on a manual machine. [EDIT: Come to think of it, there's probably a lot less heat generated by split point for the same reasons.]

Don't even think of using a dull drill bit.

Your feed is too high and your RPM too low going with 50 SFM the rpms would be 434 on the .440 drill I would go .001 IPR on a lathe so that would give you .434 IPM on a mill. Also I would at least go with cobalt and preferably
ones with (titanium nitride/titanium aluminum nitride)coating. Even with the right feeds and speeds standard bright finish high speed steel drill bits aren't going to last long in 316. Call a Guhring rep or check their website for exact recommendations if you have a lot of parts to make.

I recently found this and printed it off and stuck it on the mill. Seems to work about right for 304.
http://www.morsecuttingtools.com/Technical Data/HSS & Cobalt Drill Speed_Feed.pdf

Good advice in here but not many people have mentioned it, use a split point drill. Trying to drive a chisel point through the material will just lead to headache and burnt out drills.

I'd be at 50 sfm and 1/64 diam feed per rev pecking every 1/2 diameter.

Thank you all so much for your input, I just moved to the area my job is at and have yet to get Internet. I'm posting from my phone and will respond particularly to your posts when I get to the shop in the am, I've read all of your messages. I'll try each of your suggestions until I get this thing done.

I'm not sure what kind of drills they are that I've been using, they're so old and spun up I can't make out the script on the side of them!

Also appreciate the tooling recommendations. i'm green as hell so it's good for me to have a start as to who to contact and where I can contact good reps. So grateful to have had your time everyone, thanks again

What I see as a problem, besides the fact that 300(except 303) series stainless just sucks..

You are keeping the same feed for a 7/16 drill as for an approximately 1/8" drill.

I know a lot of the feed formulas are based on diameter, with a linear relationship, but
think cross sectional area.. A .44 diameter rod has a cross sectional area of .15 square
inches. A .14 drill, 1/3rd the diameter has a cross sectional area of .015 square inches.
1/10th the area.. Then add in all the flutes and shit.

Aint gonna work...

Then again it is a Haas, are you sure you aren't stalling the spindle with the .140 drill??

Split points in work hardening materials.. Actually split points almost all the time since I'm
not a cheap prick.. Stubby drills all the time, unless absolutely necessary.


On trying to spot with a drill.. I have no problem with that, I do it all the time, but it better
be a stubby split point, or a carbide, and you ease her in there.. Spotting with a .140 Cobalt
split point stubby in 316, maybe .0006 a rev, 50sfm.. If its a jobber, might as well just
break it in half with a hammer, and not even bother putting it in a tool holder. Might as well
just toss it in the trash if its not a split point either.

Seems to me like you are rubbing and not cutting. It would be okay if this was NASCAR (rubbin' is racin') but it's not. Spot drill it (if you got it) or center drill it (holy shit its worked for me thus far) and go to work. No need to pilot drill that small of a hole. 60 SFM and 1% of the drill diameter as the feed per revolution for starters. For your .440 diameter drill that would be:

520 RPM
.0044 in/rev, or in milling machine units, 2.2 in/min.

I fully expect you to be able up the feed by 50% once you are comfortable. Of course there are a lot of good recommendations on coolant concentration and drill point selection you need to consider as well.

bigjon61 said:

Seems to me like you are rubbing and not cutting.

Click to expand...

.004 of feed on a .140 drill, that's "rubbin'" Better feed it harder so it breaks quicker.

.004 of feed on a 7/16".... I keep forgetting.. Its STAINLESS.. Got to FEED IT even though
EVERY SINGLE TOOL MANUFACTURERS RECOMMENDATIONS have tiny little feeds for work hardening stainless.

sharp drills are a must...if you are using ragged out dull drills you might as well use just a drill blank...cause it aint gonna work. i work in the world of "if its dull just grab a new one" but i came from the world of "if its dull sharpen it"...if you dont know already, learn to sharpen drills. in cnc drilling you dont have the feel so you need to listen, if its squealing you are spinning too fast with not enough feed, if you are hearing grinding you are spinning too slow with not enough rpm...if it sounds like crackling your not getting good chip clearance as the chips are pushing around the flutes, a real good and fast way to break drills. as for coolant, have at least one nozzle aimed so that when the tool retracts it is blasting coolant right into the hole to really clear the chips out.

the small holes can be a bastard, its where tsc really earns its cost.

HideTheCarbide9 said:

I'm not sure what kind of drills they are that I've been using, they're so old and spun up I can't make out the script on the side of them!

Click to expand...

Hmm... I did say something about not using dull drill bits, did I not?

By far, the easiest solution is to purchase new drills that are designed for your application. That being said, it often isn't warranted for a one-off... but that's a fair enough sized chunk of 316 you have in front of you too. You did mention that tools are in the budget, so take advantage of that if you can.

But never forget that a good machinist can do much more with lousy tools than a poor machinist can do with all the tools in the world. I'm one of those odd ducks that actually prefers working with 304 - 316 over plenty of other carbon steels. If you know how to work it, you get amazing results with little hassle. If you don't respect the material, you get nasty results and lots of tool breakage.

I wouldn't recommend hand sharpening your existing beat-up drills as the first option, but do consider it as an option. If you don't have practice with this, or isn't someone there than can do a decent job then put it on the back burner. Stainless is not the material to start learning this with. When you're done with the stainless, start your practice sharpening and drill some aluminum or Delrin to test them out. There are lots of good YouTube videos to draw upon for this.

I often(always?) found SS plate to not drill at all like say round bar, that plate stuff often gets work hardened a fair bit, though 1" maybe ain't quite as bad as the 1/4 - 1/2" range stuff.

Bobw said:

What I see as a problem, besides the fact that 300(except 303) series stainless just sucks..

You are keeping the same feed for a 7/16 drill as for an approximately 1/8" drill.

Click to expand...

Actually, this is exactly how it should work. Caveat: because circumferential speed decreases as drill strength (capability) increases, the feed rate (in ipm) basically stays locked until you run out of rpms. Figuring out IPR is just a wasted effort, because it is constantly proportional to SFM of a given drill diameter. It looks 'dynamically variable', but it is just like embracing complexity for fun.

So for drilling mild steel with HSS drills, you'd basically use maybe 8 ipm (fairly heavy feed) all the time, so long as your SFM is staying constant (which means rpm is inversely proportional to drill diameter). The instinct to increase rpm and decrease feed is backwards (well, increase the rpm for smaller the drill, but don't change the IPM feed, because it is automatically feeding lighter in IPR). A sharp drill will penetrate 304 and 316 like crazy, if it is getting sufficient coolant. If the point is getting burned off, get more coolant down the hole, or slow down the rpm, but keep the feed heavy. Watch the chip coming up the flutes, it must come up as a continuous chip, but as soon as it stops flowing, then that becomes the peck depth.

That's my theory, anyways. Like has been said above, keep the drill sharp. If it does the squeak-crunch thing, you stop immediately and sharpen it. That is really what is so painstaking when drilling SS, is the constant monitoring of the drill sound and doing something about it when it sounds wrong. Do not cross your fingers and hope it will 'fix itself'.

Edit: discovered this constant feed in ipm thing when I was creating my tool library, and carefully entered a unique IPR for each size drill, stepping the feed up as the diameter increases. Lo and behold, when the feed rate is calculated in ipm, it was practically the same figure all the time! That was for HSS drills, drilling with 80 sfm constant.