Drilling 316 stainless steel

We are trying to drill 316 stainless steel on our CNC Lathe. It's a .250" hole x 1.5" deep.

We are drilling into 9/16" HEX.

What kind of drill should I be using, and what type of speeds, feeds, and pecks should I be taking?

I use cobalt at about 100 sfm. feed about .003 per rev. peck every dia.

We need a lot of help on these 316SS parts. We currently run 303SS just fine. But with 316SS, and slowing down the speeds and feeds, it still doesn't work right. I wear out and break inserts a lot.

I'd like to invest in new tooling.

We mostly make small pipe fittings. Our website is www.hosco.net. That will give you an idea on what we make.

I need a good roughing insert that can turn the front and back of our pipe fittings while trying to stay close to the spindle.

Then I need a finishing insert. I'd like to stay with a grooving insert that's about .100" wide.

Then I need a way to thread ID and OD threads. Right now I'm single point threading. Is that the best way?

If anyone can help, it would be great.

with 316, you can't be gentle with it- it will work harden and get very difficult.

Try 150SFM & .003IPR with a decent carbide drill. Peck as infrequently as possible.

Kennametal 9010 is a decent insert. Single point ID? You can tap if you have good results, but I hate breaking taps... Single point may not be horrible.

Not knowing your machine or seeing a print I can only provide suggestions. I did look at your site. It appears that a swiss machine would knock many of your parts out fast. I have two Stars dedicated to turning 316L, They run 24/6.

Suggestions: A carbide oil drill (for a deep hole), I use a Ghuring series 5514 (.161 dia, not oil drill, self-centering). I run at 3500 RPM , .0035 rev, .25 dp. I get about 6000 parts a drill. Also, OSG makes a drill List 1100, specially for stainless. They work great. For turning use ground inserts for finishing. I use Walter, CCGT/VBGT. I use to use molded inserts CCMT/VBMT, they don't work as well. Stainless really like to be sheared. I don't have an answer for roughing, all my turning is in one pass. For threading I use Seco LT inserts in the CP500 grtade. I get at least 10,000 parts a tip (10-32 od). I run at 2000 RPM for turning. Iternal theading I use Micro 100 with TiAlN coating. The coating doubles the tool life.

A key to turning stainless is the coolant/oil. The flash point for water based coolants is 212. For oils it gets up in the 400 range. Huge diffence in tool life.....Oh, and the high pressure coolant makes work fun (except when setting up ).

Once speeds and feeds have been figured out 304 and 316 are some real nice materials to work with. Parts come out with great finishes and burr free.

Good Luck.

Oh yeah, One more thing. I hate using Hex stock. To many irregularities, impurities and tough on inserts. I cut all my hexes with the Polygon now, much easier.

I have had good luck with colbalt drills in 316 from Nachi. A .113 dia. drill ran a couple of hundred parts drilling .450 deep. Looked like new at the end of the job. Held the size every part. I wish the taps would work that good. I would ask Sandvick for recomendations on insert grade, just cause I like there stuff and have had no trouble with most of it.

Once speeds and feeds have been figured out 304 and 316 are some real nice materials to work with.

Click to expand...

Yep.

I also use the black steam oxide coated cobalt drills made by Nachi with great results. I use the 135 degree split point drills in screw length. I found that I have to peck more often than each dia depth because the chips are very long and stringy and I end up with a birdnest that can sometimes get caught on the part.

If you are making a large number of parts and are looking for ultimate longevity of a drill, I would assume that coated solid carbide drills are the way to go.

Max

I need a good roughing insert that can turn the front and back of our pipe fittings while trying to stay close to the spindle.

Then I need a finishing insert. I'd like to stay with a grooving insert that's about .100" wide.

Then I need a way to thread ID and OD threads. Right now I'm single point threading. Is that the best way?

Click to expand...

For roughing and most finishing try this grade and style insert from Kyocera

For fine finishing use their PR930 grade PR930 Info

I recently used a VBGT insert in PR930 to finish turn 316 Stainless to a 4 Ra finish on a Tsugami.

LT, I just talked to a guy about this today. If you are buying ccgt,or vbgt inserts thinking they will cut better you are wasting the extra cash. The only purpose for a ground periphery is to make the i.c. more accurate,for indexing puposes. When you index the insert will be more close to the size you were cutting at versus a molded insert the tolerance is a little more.

nomgis - Not looking to argue....but after a year tool life study, we came to the conlclusion that the ground inserts out perfromed the molded inserts in "our application." We managed to get tool cost per part down to the mils........going from $.012 to $.005 /part, actually put cash in our pockets.

Lt, I wasn't trying to argue either,but I thought same thing about ground inserts.I was just trying to help because I know the ground ones cost more,but just like you said in your application they work better.

KennaPerfect inserts (formerly Hertel Fix perfect) are pretty neat inserts for 304 or 316 stainless. These are the 8 sided 'on-edge' inserts. I find them to be quite free cutting, and with proper feed setting, produce a nice smooth coiled chip, about the diameter of a pencil. These will break at about a 4 to 6 inch length, and are quite nice to handle and sort through, if your parts mix with the chips.

The same insert is also good for finishing with, as the positive free cutting action helps to reduce toolpoint pressure, especially on slender parts. Work hardening is minimal, as the insert has a sharp smooth rake face, and does not rely on the typical pressed in chip former. The chip former on the Kennaperfect insert is about 1/16" to 3/32" from the edge of the tool.

This insert is the closest thing in performance that I've seen compared to a hand ground lathe finishing tool, if there are any advantages to that. However, it is not good for plunge cutting at all.

Iscar Cutgrip is also a very nice tool for machining difficult 304 and 316 materials. Again, the chip former geometry is more open, requires no brute force to break the chip. But, the depth of cut is limited to some degree, depending on how rugged of a tool size you get, I guess.

You've got to get the correct insert coating for stainless, or the chip will erode a crater in the tool in no time.