ID Grooving 316 Stainless Steel

Italiano83 · Sep 6, 2016

I'm using a .070" Width ID Groover, solid carbide. ID of the bore is .734 and my ID groove OD is .819". I'm only going about .040" deep and I keep breaking these damn things after 6 or 7 pieces. A good amount of squealing going on as well. Spindle direction good. Coolant good. Currently at 250SFM and .0005"/rev. Was at 100 SFM .0015"/rev. Neither seems to get the job done. I'm not pecking, just a straight .040" plunge. Any ideas?

SND · Sep 6, 2016

Same machine that can't seem to face groove? maybe there's a common denominator... or did you figure out that issue?

Although I just play with machine lathes...
I keep solid carbide groovers(internal tool/micro 100 type) around 50-100sfm, maybe .0005-.001" feed. Those little carbide groovers don't stay sharp forever, even less so at 250sfm in 316. If doing many, maybe switch to something that takes an insert that can be changed every x amount of parts.

Usually when I've seen those or solid carbide threaders get chipped or break its a chip clearing problem though, or not enough oil/coolant getting in there.

MaxPrairie · Sep 6, 2016

What is the shank diameter of your groove tool? How much is hanging out?

Italiano83 · Sep 7, 2016

SND said:
Same machine that can't seem to face groove? maybe there's a common denominator... or did you figure out that issue?

Although I just play with machine lathes...
I keep solid carbide groovers(internal tool/micro 100 type) around 50-100sfm, maybe .0005-.001" feed. Those little carbide groovers don't stay sharp forever, even less so at 250sfm in 316. If doing many, maybe switch to something that takes an insert that can be changed every x amount of parts.

Usually when I've seen those or solid carbide threaders get chipped or break its a chip clearing problem though, or not enough oil/coolant getting in there.

I did figure out the face grooving issue. I need to go update that post. The insert geometry the way its made has zero relief on the bottom edge, so it theoretically drags and if a chip snags it, its done. I had to put a 5 to 10 degree angle on it and now it cuts like butter.

As far as this internal groove goes, I'm going to bump my sfm way down like you suggest and add an additional coolant nozzle coming in at a different direction and see if that helps. Its a pretty beefy groover, at .375" shank and .070" width with minimal projection, something like .090".

SND · Sep 7, 2016

Is it breaking while its cutting or is the groove to its final depth on the last part when the tool/cutting edge breaks?

apoc_101 · Sep 7, 2016

Use a narrower grooving tool for less deflection. .047" maybe. rough the groove with partial depth, move on Z, peck to same depth, then continue your way down... then finish the width and depth of the groove with a few thou to come out.

aj · Sep 7, 2016

First, I'm not a tool salesman or tool rep. I just machine a lot of 316. So this is just my $0.05 worth...

We do a lot of I.D. grooving on 316, hundreds of pieces at a time. I've grown kind of fond of Kyocera I.D grooving tools myself. The one I'd use for your application is a SIGER08-10C. It's through-coolant and has a 0.062 insert width. Choke up on it as much as you can-don't leave too much hanging out.

I think your 0.0005 feed rate is giving you a work hardening issue. Try upping your feed to around 0.002/rev.

chip_maker · Sep 7, 2016

Try checking your radial turret alignment.

Also radial relief on the groove tool. Too much tool pressure could be causing them to break.

Search

Largest Manufacturing Technology Community on the Web

Search

ID Grooving 316 Stainless Steel

Italiano83

Aluminum

SND

Diamond

MaxPrairie

Hot Rolled

Italiano83

Aluminum

SND

Diamond

apoc_101

Hot Rolled

aj

Hot Rolled

chip_maker

Stainless

Similar threads