Drilling 304 Stainless Steel

MetalWorkingFAQ.NET · Nov 6, 2009

Hi everyone-

We have been having serious problems drilling both 3/16" and 1/4" holes in 304 stainless using the following: HSS, HSS TiN, Cobalt, Cobalt TiN, Cobalt TiCN, Cobalt TiALN drill bits in both sizes at a depth of 1" (effectively 5.3X and 4X) with speed/feed of 1018RPM/3IPM for the 3/16" for example. We're flood cooling and using a VMC to do this. Bits burn up, die, work-harden the hole and we're SOL. Using the CNC, we used a peck drill of .1875 and it worked fine for a test piece and then in the actual customer piece, the first holed failed.

Doing this manually yields better results. In fact, manually, using the 1/4" cobalt bit with 118degree point works the best. The chips need to be cleared after every plunge from the flutes and the hole and bit need to be generously re-lubed, but it's yielded the best results (i.e. holes can be drilled at least...) so far. I

Two questions:

1. Using CNC, what would you all recommend?
2. With the tip of one of the 3/16" bits in a hole that didn't make it, how can we extract it? It needs to be a through hole. EDM?

Thanks!

landm1 · Nov 6, 2009

304 stainless.

Some small things you might have already tried.

132 degree splitpoint drills. On a standard 118 deg drill the web creates heat, not big help in 304.

On holes that deep keep your peck depth light, it works for us in the short run stuff.

Do not wait for your tool to break before you change them. Establish a minimum tool life and do the math on your profit.

Check the condition of you coolant, bump up the concentration.

If you are doing high production try through tool collant, high pressure. We use standard coolant pressure in our spade drill, they are great.

On larger stuff we are having real good luck with spade drills and insert tools, no peck. I think the hole trick is to flush out heat with the chips.

To remove broken stuff in holes I keep old torn up carbide endmills. But 1" deep with a .25 drill is a bit of a reach.

Oh well, I am sure someone around here does stuff like that for a living.

LandM-1

MetalWorkingFAQ.NET · Nov 6, 2009

Thanks for your comments. We have used only the 130 and 135 degree points. Funny thing is that the best performing bit/usage has been the 1/4" 118degree cobalt fed manually.

We didn't increase the coolant concentration.

A tool vendor mentioned using no peck but dwell instead. His rational was that it was important to make sure no chips stayed in the hole.

I'm tempted to just go with those OSG EX-SUS bits and follow their instructions. At $20/bit it's expensive, but if the problem's solved, then it's well worth it.

Still, what can we do about the bit that's stuck in the hole?

BobWarfield · Nov 6, 2009

Looks a touch fast for a Cobalt.

Precision Twist has some guidelines for deeper holes that I used for my G-Wizard Machinist's Calculator:

http://www.precisiontwistdrill.com/techhelp/article08281995.asp?image=contact

If you apply those, your numbers would look more like:

35 SFM / 700 rpm

1.71 IPM

Just a thought.

Best,

BW

G-Wizard: http://www.cnccookbook.com/CCGWizard.html

Chobyn · Nov 6, 2009

I have had good luck with 135* split point cobalt drills in 304. You might want to check what tool you are using to spot or center drill with as well. It might be hardening up the initial hole start and undermining the next tool.

~1/3 the drill diameter is what I use for the peck amount. Keep the cutting edge of the tool cool and it will be a much happier tool

I am guessing that with your manual feed comparison that your peck is much less than the .1875 you specified in the original post.

I completely disagree with the dwell idea with 304.....the last thing you want that cutting edge doing is idling(rubbing) against a work-hardenable material. If it isnt 'in the cut' get it off the material.

To get the broken 3/16 drill out...depending on how far the drill got BEFORE it failed, I would try a re-grind 3/16 em (.177 or smaller) carbide 4flute end mill to get it just past the work hardened area. This is going to kill at least one end mill, by the way.

Good luck!

Troup · Nov 6, 2009

MetalWorkingFAQ.NET said:
A tool vendor mentioned using no peck but dwell instead. His rational was that it was important to make sure no chips stayed in the hole.

Only if your machine and setup are extra-rigid.
Otherwise dwell will workharden like crazy :willy_nilly:

Even with a rigid situation, I'm not sure it's a great idea.

I think pecking with an air blast on retraction would be better if you have that facility

MetalWorkingFAQ.NET · Nov 6, 2009

Chobyn said:
I have had good luck with 135* split point cobalt drills in 304. You might want to check what tool you are using to spot or center drill with as well. It might be hardening up the initial hole start and undermining the next tool.

~1/3 the drill diameter is what I use for the peck amount. Keep the cutting edge of the tool cool and it will be a much happier tool I am guessing that with your manual feed comparison that your peck is much less than the .1875 you specified in the original post.

I completely disagree with the dwell idea with 304.....the last thing you want that cutting edge doing is idling(rubbing) against a work-hardenable material. If it isnt 'in the cut' get it off the material.

To get the broken 3/16 drill out...depending on how far the drill got BEFORE it failed, I would try a re-grind 3/16 em (.177 or smaller) carbide 4flute end mill to get it just past the work hardened area. This is going to kill at least one end mill, by the way.

Good luck!

ahh. the dwell issue makes sense.

as for the peck drill depth in the vmc, i used the diameter of the drill. so, .1875... strange that manual feed seems to get further than drill diameter. the method i used with the manual mill was to apply steady and increasing pressure until i saw smoke rising from the tapmagic fluid

then withdraw the drill, apply a steady stream of said coolant back into the hole and on the bit. i stop the spindle, manually remove the stuck swarf from the flutes of the drill bit (talk about not efficient) and the proceed again. this method has been the most effective...

as for the removal of the bit, i'll try the end mill method. no worries about killing an em. if it works, it'll be a time saver for sure!

MetalWorkingFAQ.NET · Nov 6, 2009

Troup said:
Only if your machine and setup are extra-rigid.
Otherwise dwell will workharden like crazy
Even with a rigid situation, I'm not sure it's a great idea.

I think pecking with an air blast on retraction would be better if you have that facility

our machine doesn't have the air blast, so i think an option would be to retract rather high above the workpiece, slide hold, stop spindle/flood coolant, inspect the flutes of the drill bit and clear swarf if stuck, then proceed again for each peck. there must be a better way!

Limy Sami · Nov 7, 2009

MetalWorkingFAQ.NET said:
Hi everyone-

Bits burn up, die, work-harden the hole and we're SOL.
Two questions:

Thanks!

Classic symptoms of wrong speed & feed.

Slow down speed to app 50ft/ min

Feed at .006 - .008 / rev.

Flood coolant.

Peck at a max of every 1 dia.

Mike C. · Nov 7, 2009

"Bits burn up, die, work-harden the hole and we're SOL."

"Classic symptoms of wrong speed & feed."

Yup, speed burns, feed breaks. Spindle speed is about twice too fast. Drop the speed and up the feed just a touch. Try to keep the feed high as possible without wringing off a drill or splitting one. High feed rate keeps the drill cutting in fresh material to prevent work hardening.

304 is a PITA on any internal work (drilling, reaming, tapping). See if the customer can live with 303 instead. If so, it'll make your life MUCHO easier.

jim rozen · Nov 7, 2009

*Way* too fast. Stainless does not have any thermal conductivity to speak of
so you need to run a lot slower than you think. Drop the suggested speeds for
the material and tooling, in half and start there.

How deep is the hole? You should be able to do it in one shot with a guhring
parabolic flute high cobalt drill. That is the tool of choice if I were doing this.

What is the "flood coolant" you speak of? Again if I were doing this, I'd use
lard oil/kerosene, 50/50 mix. That's probably not compatible with your machine
but you need to specifiy what you are actually using so folks can examine the
choice.

Jim

Mike C. · Nov 7, 2009

"Stainless does not have any thermal conductivity to speak of..."

Indeed, Jim. That's the root of the problem. Stainless and titanium both do this. They are poor conductors of heat, so instead of spreading out into the workpiece, the heat runs right back up into the tool, path of least resistance. In addition, this causes the tool to expand and can cause problems with the finish in a drill as the periphery rubs, or cause it to bind up and wring off, as with taps and reamers with have more area contact. I have had many taps wring off in titanium when backing out.

MetalWorkingFAQ.NET · Nov 7, 2009

thanks for the replies all.

here's what i did today:

(no CNC, all manual)

touch up the cobalt tin and tialn bits in the drill doctor after each 1" hole (for the 3/16" dia.). thanks to bob for reminding me that this is considered a "deep hole".

i noticed that i could feed the drill in about .2" or so on each pass. the chips were long/stringy and didn't evacuate from the flute. i think in the cnc situation (speed/feeds adjusted) the chips still don't leave the flutes, making NO room for the next peck. also, i think that upon peck, there should be an extra second or two where the drill bit can be cooled down and gives plenty of time for coolant to enter the hole.

as for the actual coolant name, i'll get a name tomorrow. it's mostly suited for aluminum and non-ferrous, but the pail does indicate that with another ratio, it can be applied for stainless.

does anyone have any recommendations on successful types of bits in addition to speed/feed? i see varying numbers all over the place.

thanks!

SDConcepts · Nov 7, 2009

we drill 1/4 holes in our cnc all the time in stainless 304. we run our coolant concentration around 12 on the refractometer. also we use 1000 rpm and .003 ipr. the first peck is the drill diameter plus half, then the drill diameter on all subsequent passes. we usually get 300-400 holes from a cheap 4 dollar cobalt drill. we recently tried an inox drill in 304 stainless steel and we are getting close to 400holes but that drill is 30 dollars. however that one we don't peck only push straight through so it saved a bunch of cycle time.

MetalWorkingFAQ.NET · Nov 7, 2009

deburring 304 stainless drill blowout?

on a similar topic, what do you guys use to debur the backside of the hole? the standard deburring tool doesn't quite do it, there's a lot of material there....

Limy Sami · Nov 8, 2009

Single flute or ''hole'' flute CSK bit.

rockfish · Nov 8, 2009

MetalWorkingFAQ.NET said:
on a similar topic, what do you guys use to debur the backside of the hole? the standard deburring tool doesn't quite do it, there's a lot of material there....

That's a very good indication that your speeds and feeds are too high. Your blasting through the back end of the part and not giving it enough time to cut as it breaks through, causing a large burr to deal with.

Frank

www.randolphmach.com

MetalWorkingFAQ.NET · Nov 8, 2009

rockfish said:
That's a very good indication that your speeds and feeds are too high. Your blasting through the back end of the part and not giving it enough time to cut as it breaks through, causing a large burr to deal with.

QUOTE]

yeah, i was concerned that the bit would somehow "catch" and break near the 1" depth. with the screw machine length drill bit, the flute length was only 1 1/8" and i didn't want any chips to cause more problems.

on one of the holes (lucky it was a through hole), i drill the other side manually until it hit the other drill bit plug, then proceeded to drive it through the hole with a punch/hammer and press. not fun at all. :O

strange that i got those speeds/feeds from the machinery handbook for hss in 304ss, proceeded to up those numbers based on precisiondrill's website indicating increased speeds (80%) and feeds (30%) (this was before seeing the post about deep hole drilling).

i'd still like to try those ex-sus gold bits from osg. there's a cool video from them on youtube: http://www.youtube.com/watch?v=YVC-uqFg7yo

Spelunker · Nov 9, 2009

MetalWorkingFAQ.NET said:
A tool vendor mentioned using no peck but dwell instead. His rational was that it was important to make sure no chips stayed in the hole.

Dudes trippin'....I have NEVER had luck dwelling on 316/304ss It work hardens the crap out of it. :bawling:

Mike C. · Nov 9, 2009

General wisdom on HSS in stainless is run at half the speed for steel (60-100ft/min). 500rpm for .500" diam gives you about 70ft/min. That would be 1000rpm for a 1/4" bit in steel. 500rpm for 1/4" in stainless. Start there, you might be able to bump up a tad, but watch the corners of your drill lips. If they start darkening, wearing or simply melting you need to back it off. Speed burns.

The coatings will help with chip adherence problems, but a thin coating isn't going to save your drill from burning up if it is run too fast.

Drilling 304 Stainless Steel

Plastic

Cast Iron

Plastic

Hot Rolled

Cast Iron

Titanium

Plastic

Plastic

Diamond

Diamond

Diamond

Diamond

Plastic

Stainless

Plastic

Diamond

Titanium

Plastic

Aluminum

Diamond

Similar threads