303 stainless work-hardening

Well, I've never had this happen to me previously on 303, only on 304. Guess I haven't really lived...

I have a 303 part in the lathe that needs a precision shaft bore for a gearmotor shaft, and it looks to me like it work-hardened when I was drilling it out (I guess). I've been trying to get a carbide-insert boring bar to bite into into it, and I am seeing serious bell-mouthing, almost out to my .750 finished bore size. The bore is 1.25" long. The hard part is in the middle and back of the part, and I just thought I would canvass here to see what options there are. Things I have considered:
-- Grinding the zone out, but no tool post grinder. Have to use a Dremel, unfortunately. No idea how deep the hardened layer is (anyone?)
-- Making the part again. (lousy option)
-- Carbide reamer (also lousy $$$, and might get jammed in the hard part and then it's back to re-making the part)
-- Bore larger and sleeve, presents some complication with finishing the part.
-- Some magic suggestion from someone that works immediately and perfectly.(My favorite)

This is a single part, which is why I'd like to save it. I have a second mating part as well, that is 2+" long with same operation, and then I need to broach a keyway in both.

How big (dia) is the boring bar you're using? Do you have a solid carbide bar? If not, can you make one from an old carbide endmill of at least .625 dia?

Gordon -- Thanks for knowing where to turn the light on inside my head. A 1/2" 4-flute carbide endmill worked perfectly, and saved the part. The insert boring bar I was using was 1/2" diameter, which I would have thought would be fine normally, but it just ended up skating over the hard part using a CCMT insert with a little radius on the corner....

Many thanks for the suggestion!

Any chance it is just poor quality 303?

Dualkit said:

Any chance it is just poor quality 303?

Click to expand...

Or too much edge prep (or bad orientation) on the boring bar insert.

specfab said:

Well, I've never had this happen to me previously on 303, only on 304. Guess I haven't really lived...

I have a 303 part in the lathe that needs a precision shaft bore for a gearmotor shaft, and it looks to me like it work-hardened when I was drilling it out (I guess). I've been trying to get a carbide-insert boring bar to bite into into it, and I am seeing serious bell-mouthing, almost out to my .750 finished bore size. The bore is 1.25" long. The hard part is in the middle and back of the part, and I just thought I would canvass here to see what options there are. Things I have considered:
-- Grinding the zone out, but no tool post grinder. Have to use a Dremel, unfortunately. No idea how deep the hardened layer is (anyone?)
-- Making the part again. (lousy option)
-- Carbide reamer (also lousy $$$, and might get jammed in the hard part and then it's back to re-making the part)
-- Bore larger and sleeve, presents some complication with finishing the part.
-- Some magic suggestion from someone that works immediately and perfectly.(My favorite)

This is a single part, which is why I'd like to save it. I have a second mating part as well, that is 2+" long with same operation, and then I need to broach a keyway in both.

Click to expand...

more about DOC, feeds and speeds and as posted above setup?

Some of the other info, for post-mortem analysis:
The manual Clausing lathe is not equipped with flood coolant, so I am using Rapid-Tap (brush and squirt bottle) which seems like a decent general-purpose oil-type lube. Sometimes I mix it with isopropyl alcohol for some additional cooling properties, but that really reduces the lubricity. The lathe does have a bed turret which helps a lot with drilling work.

I had to turn part of the length down to 2" from 4". Lots of stock removal, repeated passes maybe .06-.08 depth of cut, .003 per rev feed rate using a CCMT general-purpose insert for steel, just warming up the part pass by pass, then I drilled out the center with a 1/2" cobalt split point drill. THEN I drilled out the center hole to 11/16 which I think may have caused the work-hardening on a part that was already pretty warm. The hardened zone was essentially in the center of the part mass, which makes sense as that is where the heat would have been mostly generated, and which has the longest path to dissipate. I DID take pains to drill aggressively to try to avoid dwelling and over-heating, but it may simply be that there was already too much heat stored in the part.

The boring bar has a "preset" orientation from flats on the shank. I was trying an up-sharp aluminum finishing insert to start with for taking "light" passes to see what sort of finish it would leave, but as noted, that insert has about .015 radius and ended up just riding up over the hard part. Tried the CCMY steel insert also, but still no-go. The dead-sharp endmill corner worked very well, problem solved.

If it happens again on the second part (even longer bore) at least I have a known solution.

Thanks again to Gordon for the dope slap;-)

Dualkit said:

Any chance it is just poor quality 303?

Click to expand...

Good question. It came from McMaster (with CERTS!), but it does seem on the 2nd part that there are obvious non-uniformities along the length when I am reducing the diameter for about 1.5" length. Definitely seems to be hardness variations.

You're quite welcome. Glad it came out alright.

Might try a smaller pilot so that your 11/16 drill has enough work to do. But it’s just one part and now you know how to fix it.

I like threads like this they help to reinforce things so I might remember the answer when I need it.

specfab said:

Good question. It came from McMaster (with CERTS!), but it does seem on the 2nd part that there are obvious non-uniformities along the length when I am reducing the diameter for about 1.5" length. Definitely seems to be hardness variations.

Click to expand...

I dont cut a lot of 303 these days but we never seem to like it. Every time it is something different. Hard spots seemed to be common.

I was going to suggest a sharp HSS bit to save money. Looks like you got it covered. I never use carbide but I know its not as sharp as HSS and my friends who use it tell me it makes cutting SS seem gummy. I never noticed it in my world, but I always have great luck with sharp HSS-CO and brand new cutting oil.

I think a lot of the 300 stainlesses have become pretty random in properties as supply has moved from domestic or good quality foreign mills to "budget" mills in East Nowherestan. Essentially shiny A36...

coolant on stainless is KEY. to success, I have a pressure sprayer for drilling on the lathe and mix up a small amount and spray it on and in the hole on the manual lathe. Hard and fast is key as its super gummy. Ive dealt with hardened stainless that just squeals after being plasma cut, it needs a harder grade of stainless insert with a sharp chip breaker to get through a hard layer of essentially carbide vs carbide. once through and kept cool, its like butter.

BT Fabrication said:

coolant on stainless is KEY. to success, I have a pressure sprayer for drilling on the lathe and mix up a small amount and spray it on and in the hole on the manual lathe. Hard and fast is key as its super gummy. Ive dealt with hardened stainless that just squeals after being plasma cut, it needs a harder grade of stainless insert with a sharp chip breaker to get through a hard layer of essentially carbide vs carbide. once through and kept cool, its like butter.

Click to expand...

This, Yeppers that is what I was taught. don't try sneak up on it .010-.015 minimum final DOC

Thanks to everyone who commented. Just a post-post-mortem note:
In doing the second part, I cooled the part a bit after turning the stock off the 2" diameter section, then really paid attention to keeping the 1/2" drill cool, then actually worked out the SFPM value for the 11/16" drill. Turns out I was way strong on the RPM for that drill size, at 350-360 RPM. That's about 75 SFPM, which is likely the reason the material heated up enough to harden in the middle of the bore. I was lazy, as it was the bottom of the open belt RPM range on the lathe, and it "felt OK". LESSON LEARNED >>>Check the numbers, don't be lazy, use back gear.

does temperature have anything to do with work hardening in stainless?

dian said:

does temperature have anything to do with work hardening in stainless?

Click to expand...

it's more of like burnishing, the surface is not cutting of it's to low DOC, for example taking .0005 DOC, the tool no longer can
cut and is rubbing both damaging the part and the tool. , I was taught to take .010-.015 DOC for the final pass
holding .001" diameter tolerance. every ones mileage will every, because the tool geometry, feeds and speeds,
the setup, rigidity , and more.
while I did not machine or program parts in the later years I worked with very experience programmers, who would cut Inconel 718 &
other high temperature alloys and at the roughing because of very rigid lathes with crazy horse power, could easily take crazy DOC
at roughing SFM and the material would fly off like butter. very impressive.

dian said:

does temperature have anything to do with work hardening in stainless?

Click to expand...

That's a good question. I may be conflating the symptom (over-heating) with the actual mechanism of work-hardening. Keeping the temperature down of both the material and the cutting tool does help prevent work-hardening due to dulling and rubbing of the cutting tool, I think, but the heat may simply be the tell-tale sign of hardening in process due to other factors.

Well, you can work-harden 300 series stainless in freezing temperatures, and you can't harden it by heating and quenching so like specfab, I suspect the heat component is most likely to affect the cutter. Its always downhill from there!

303 stainless

Have you tried 303 with selenium in it? Entirely different animal.