Drilling Stainless 316L

[Stoneair666]

Having problems with tool wear drilling stainless steel 316L.... First time working with material, i need experienced advice....

[Karl_T]

Less speed, more feed. Keep tooling extremley sharp. Some prefer oil to water based coollant.

316 work hardens easily. Once you've done that, you're screwed.

316 is just like 304. Machinst mantra:

304 she's a whore
303 she's for me.

Karl

[Stoneair666]

cool, well to get a little more detailed i'm drilling .218 dia to a depth of 1.250. Turning at about 600 rpm at 2.5 feed pecking at .015 like i said it is my first time working with the material, and it's driving me nuts, i think my shop accepted the job of 3000pcs without realizing how difficult it is to machine this *****. Endmills i got cutting it like butter. the drills i am using right now are cobalt, i think they're **** and am waiting for tooling from osg, the ex-gold. Am i hardening my part drilling the way i am drilling? i get 15-17 pcs before my drill wears out.... 2 holes each peice i get approx. 30 holes done per drill.... i know somethings wrong but i am the only machinist in my shop so help is hard to find and previous guy never had the oppritunity of working with 316L.

[Karl_T]

This is terrible, I've only been machining for 30 years, and I've never memorized a speed or feed. I just go by how it looks and feels. Sorry.

Look at the chip. it should look too thick for steel. A broken workhardened drill will be chipped on the outside shoulders of the drill. The outside edges of the drilled hole will look shiny. You've got a lot of parts to do, I'd try increasing feed at your speed first. When you snap a drill in the middle, your feed is too much <Grin> I hate the oil mess, but it would increase your drill life.

You're not going to get long drill bit life, but you should be able to do a bit <pun> better than that. You might try split point drills.

On large holes, I've used the raycon point with GREAT success. Gets rid of the shoulder chipping and dulling.
http://www.winsloweng.com/articles/g...rm_content.htm

On usenet, you might ask your question on alt.machines.cnc. Theres folks that hang out there that have the speed and feed memorized for any cutter and any material.


Karl

[Karl_T]

Originally Posted by Karl_T Look at the chip. it should look too thick for steel. A broken workhardened drill will be chipped on the outside shoulders of the drill. The outside edges of the drilled hole will look shiny. You've got a lot of parts to do, I'd try increasing feed at your speed first. When you snap a drill in the middle, your feed is too much <Grin> I hate the oil mess, but it would increase your drill life. Karl

P.S. If your drilled material comes out a burnt orange color, you're going too fast. Drill is going to toast real quick.

[lakeside]

.218 drill 960 rpm 3.3ipm peck of .1 not .015 at that peck depth you are work Harding the part by the time you drill start to cut you are retracting and starting a new cut this is just build heat and burning drill for feeds and speed check out the site for ME pro it a data base for feed and speeds I posted it the past and this is a question that keep popping up the software is $100 but you will save that on burned out piece and part in no time

http://www.mrainey.freeservers.com/

[HuFlungDung]

Lakeside makes a valid observation about the peck drilling depth being too shallow at .015"

Cobalt drills (or better) are almost a must because of the extreme heat concentrated in the cutting zone (stainless is a poor conductor). I've also experienced a moderate improvement in drilling performance by using a fast spiral drill. A travelling salesman for Dormer tools happened to show me a set of these and I was impressed.

Flood coolant is mandatory, IMO. Without it, you'll have to slow way, way down.

Inspect the tool frequently for damage. You want to know what really makes a hard spot? When the first 1/4" of your drill is glowing red in the hole That would be HSS fused to your plate.

[fpworks]

I have had fairly descent luck with work hardening material using solid carbide drills without pecking. (punch straight through)

Justin

[lakeside]

Originally Posted by fpworks I have had fairly descent luck with work hardening material using solid carbide drills without pecking. (punch straight through) Justin

That may be true to a piont(if you want to work hardend part I think you ment without work hardeding of part just the wise guy in me) no more than the drill dia to depth ratio but if your cutting to a depth of 1.25 you need a peck stainless needs to be cut some what aggressively I like to use 1/2 of drill dia. as a starting point for peck depth

[fpworks]

Mike,
You don't always have to peck drill deep holes ;-) The trick here is to do everything possible to avoid work hardening.

With solid carbide drills, it is generally recommended to not peck.

If I were doing Stoneair's production job (dia 0.218", depth 1.25", 316L stainless) the first tool that I would set up with would be a solid carbide drill with a 140 deg point, no pecking, and no spot/centering for hole start.

Maybe this will work for him, especially considering the time savings with production work.

Now, the peck depths are too shallow, so there are too many pecks. Each time you peck, the drill is having to punch through the hardened surface, so this is why the tool wear is so high. If the pecks depths were deeper, then there would be fewer instances where the drill tip has to punch through hardened material.

[lakeside]

yes I can agree on some of the point but I will use a peck if for no other reson than keep the chip lienght down so as not to wrap around spindle and to clear hole I also feel that the time that added by a peck can maybe save you from changing a drill the time would be the same in the end as alway we try to cut as fast as the aplication will handle carbides can be the best way to go but still if your down 1.25 your chip is going to be quite long I will agree on the 140 piont also I like the split piont

[lakeside]

......................................................................................................................