Recommended feeds and speeds for drilling 316ss??

[tgmcg]

I've got a Shizuoka AN-S knee mill with 3HP spindle motor Centroid CNC controller. Have been using it the past 2 years mostly for aluminum work.

My requirement is simple. I want to drill 1/8" dia holes in 316ss rod or plate up to 0.625" deep as quickly and reliably as possible.

Am currently doing this with spindle speed of 1000 rpm and 0.2 ipm feed rate using a carbide tipped drill and Tulco coolant.

Would be grateful for any specific guidance you may offer.

Best regards,

Tom

 

[metman]

Tom,

1,000rpm would work with High Speed Steel drill bit. You can rotate much faster with carbide but I will have to look it up at work in my machining data handbook. Are you sure your drill bit is only tipped or is it solid carbide? If only tipped, I suggest you go with solid since you want to minimize deflection of the bit for the following reasons: 1) S.S. readily work hardens and therefore you want good feed rate (I will also look this up) so that you are cutting thru the material rather that working it. .2ipm at 1000rpm is .0015" chip load for two flute drill which might be ok but guessing it should be a little more for S.S. 2) Carbide is much stiffer than steel (about 10 times I think) and therefore will deflect less for a given feed rate giving you a straighter hole since you are driving a bit or column with a large slenderness ratio.

Faster rotation will also promote better chip removal for your realtivley small diameter.

Also suggest you use peck drilling to clear chips and provide for entry of coolant.

Jesus is THE life,
Leonard

 

[tgmcg]

Leonard,

Thank you. This is such a great site with so many very knowledgable people.

Yes, the bit is only carbide tipped as I was concerned about breakage...perhaps overly concerned. As most of these holes are in 0.500" dia 316ss shafting, I use a centerpunch to mark the hole, and also use a G73 peck drill cycle with 0.015" depth per peck.

Drilled a couple of holes last night at 0.4 ipm with no obvious problem. Still seems awfully slow. I can hack off a piece of 0.500" dia shafting with the bandsaw in maybe 30 seconds, vs several minutes to drill a hole. Seems there could be a mismatch there.

My main concern being a relatively new machinist is whether or not I'm way off the mark on the slow side regarding the feeds and speeds. So much about the art of machining seems to be passed by word of mouth only.

Best regards,

Tom

 

[metman]

Tom,
If I read you correctly, you were still using 1,000rpm with the increased feed rate of .4 ipm?

Sorry I did not get back to you with the info. I thought about your post at work and almost stopped for a few minutes to look it up and then got very busy again real quick if you know what I mean.

I am fairly certain you can boost the rpm and consequently the feed rate. For a starting point, I typically run carbide cutters 3-5 times the rpm that I would use for the same material/setup vs High Speed Steel cutters.

So if you have a spare carbide tipped drill bit, you could try running at 3,000 rpm/1.2 ipm on a sample workpiece. But again with the higher feed rate your chances will be better with a solid carbide drill for rigidity.

Hope this helps.

Jesus is THE life,
Leonard

 

[metman]

Tom,
My machinining data handbook predates carbide drill usage but we have some up-to-date info at work:

We purchase small daimeter solid carbide circuit board drill bits for drilling holes in Aluminum sheet. These bits are typically shorter than stub drills and therefore even more rigid. The manufacturer recommends the following for 1/8 dia in 300 series S.S.:

200fpm and .0012ipr So yes you are way low on both rpm and feed rate.

(200ft/min)X(12"/ft)X(1rev/.125pi) = 6112rev/min
X .0012in/rev (ipr)
--------------
7.3 ipm

At this feed rate you should go thru 1/2" thickness in about 4 seconds discounting peck time.
.5/7.3 = 0.068minutes, .068X60 = 4.1 seconds

Or another comparison is 7.3/.4 = 18 times faster than your last reported try. You said it is taking several minutes. 120seconds/18 = 7seconds.

Do these numbers suggest an investment in solid carbide drill bits?

Jesus is THE life,
Leonard

 

[unclesyd]

No one has mentioned that it is extremely important to keep everything rigid,especially the work piece. Make sure the lock, if you have one, on the table is holding the table rigid. Look at the different styles and coating for carbide drills. The performance of carbide can vary significantly with each setup and material.

Here is website that has a handy calculator for drills as well as other good information.
The original poster of the URL shall remain anonymous as I’ve lost my list.

http://www.carbidedepot.com/default.asp

 

[tgmcg]

Thanks Leonard.

The max spindle speed for my mill is 3550 rpm, so can scale down the feed accordingly.

Most of the holes I'm drilling are through-holes for 0.125" spring pins in 0.500" and 0.625" shafting, so there's the problem of keeping the drill centered, which is why I use a cenerpunch to mark the hole and then jog the mill into alignment before drilling.

Shorter bits sounds like a great idea. Will buy some.

Do you have any concerns about my use of the Tullco Polycut water-based coolant?

Regards,

Tom

 

[tgmcg]

Many thanks for the link, unclesyd.

My CNC mill table does not lock. The Shizuoka is a pretty beefy and rigid machine as far as kneemills go. I generally clamp the ss shafting in a v-block which is held in a mill vise, and then drill into a short (1.000") cantilevered section of shaft. However, I see no reason why drilling into a fully supported section of shaft wouldn't work.

Will definitely pay closer attention to set-up rigidity when using carbide tools.

Regards,

Tom

 

[metman]

Not familiar with your particular coolant. There are so many different kinds and some are very good. Maybe what you are using is just fine?

for Steel and S.S. I like the black resulferized cutting oil like Rigid supplies for pipe threads. But try your max cutting speed with proportionate feed rate as you intend without changing cutting fluid so you can evaluate one variable change at a time.

If you give this thread some more time hopefully someone will respond with some expert advice on coolant or maybe even corroborate my choice.

Jesus is THE life,
Leonard

 

[mrainey]

I've never had much luck drilling deep holes (five diameters, in your case) with carbide twist drills, except in non-ferrous materials and cast iron. I've found that as the drill goes deeper, that chips tend to eat the carbide up. If you do a lot of pecking and withdrawing, the problem of thermal shock comes into play if your drill doesn't have thru-coolant. Particularly on a vertical machine, rapiding out of the hole then back in increases the chances of running into packed chips, resulting in damage to the drill.

I'd look at some of the newer coatings on a HSS drill for deep holes in stainless. Reasonably high surface footage combined with a tougher drill.

 

[tgmcg]

Leonard, thank you. Since I use the one machine for a variety of materials...mostly aluminum, I prefer to stick with one coolant.

Mrainey: Comments duly noted re: deep holes. I've been using a pretty short peck of 0.015", withdrawing maybe 0.100" after each peck. I suppose shortening the withdrawal distance to say 0.050" would also speed up the drilling process considerably.

Many thanks,

Tom

 

[bill1898]

Tom, I agree with a lot of what has already been said. As already mentioned, 316 work hardens quite rapidly when a tool is creeping along, or allowed to dwell. For that reason, the most important thing is for you to keep that tool moving ahead as rapidly as possible within the constraints of the operating conditions. The chip load on each flute should be at least 0.0015 inches. This means a penetration rate of 0.003 inches per revolution of the spindle. At 1000 rpm this gives you a penetration rate of 3.0 inches per minute. For the 0.625 depth you mentioned it would take 12.5 seconds to penetrate through the part. The drill may not be able to take this, but, if you have to decrease the inch/min rate you must DECREASE the rpm accordingly to maintain the chip load. The actual processing times will be longer, of course, depending when you start the feed mode of the spindle. If the drill is sharpened properly I question the neccessity and value of the peck feed function. Also, with a carbide drill, coolant may do more harm than good. However, if coolant is used and it can be directed to where it is needed, a low coolant to water ratio may help get the chips out. Hope this helps.

 

[tgmcg]

Bill,

Thank you. I'll be drilling some more holes today and will crank the feedrate up. I was given the 0.3 ipm by a deep drilling contractor. Sounds like either they were way off or I totally misunderstood...probably the latter.

I understand about the work-hardening issue. We'll see if my 1/8" drill bits can withstand the load at 3 ipm. Will vary speed as necessary to maintain constant chip load.

Working with aluminum most of the time has obviously spoiled me. (g)

Best regards,

Tom

 

[doctorinthehouse]

I found that using guehring s-drills work really well in 304 and 316. try it !

 

[surfdog]

McGuinness,

I know this is a few months late but use an OSG EX GOLD DRILL.....made by OSG......they are amazing......we make a particular part here at work from 316SST with approx 400 holes in it (looks like a pasta strainer) and those drills do a great job....without a burr on the "break thru" either...not spotting and no pecking....you will be amazed.....I was skeptical at first but now I use them on every SST job I can....good luck

Kevin