Cutting 4140 heat treated to Rc 50-55

BRIAN.T · Sep 14, 2020

I don't think I've ever cut heat treated 4140. How difficult is this condition to work with? The part isn't too complicated, it's got a few +/- .002s on it.

Thanks

1953chevB · Sep 14, 2020

BRIAN.T said:
I don't think I've ever cut heat treated 4140. How difficult is this condition to work with? The part isn't too complicated, it's got a few +/- .002s on it.

Thanks

very slow going, turn and mill?

BRIAN.T · Sep 14, 2020

1953chevB said:
very slow going, turn and mill?

That's about what I expected. It's 95 percent turning, a small milled feature at the end.

Except for it being slow is it relatively predictable? Or am I to expect irregular tool failure?

Phil in Montana · Sep 14, 2020

Harder than the hubs of hell, It can be done with costly bits but worth the fight.....machine the part and then heat treat...Phil

CarbideBob · Sep 14, 2020

You do not mention what type of tooling you have.
HSS, not so good.
I generally rough oversize, then heat treat, and finish by grind, or hardturn/hardmill with cbn, cermet or a really hard carbide grade.
It distorts in HT so at .002 I do not think you can go to finish size in the soft machine ops.
With enough samples run you can overcome the grow/shrink but you can't do anything about the warp.

Cbn by far the most predictable for hardturning and fast but $$, C6-C7 coated carbide for endmilling. If the milled feature can use a face mill, again cbn or cermet.
Tools must be pulled before they dull, try to push the life and things become a mess fast. Worn out tools here look like they have barely been run on the flanks under a magnifying glass or loupe.
We save the endmills and reuse them on softer steel. We color the ends blue before they go back into the tool drawers which means "lightly dulled".

We make our fixtures for holding large run carbide inserts on the grinders in this range for longer life and occasionally run into a toolholder or cartridge that the customer wants in this range.
It is a learning experience and expect some real frustration at first. Mid 40's is easy peasy falling off a log compared to this.
First time I tired I failed so miserably, broke everything over and over. Began to think it was just this side of impossible.
Dad, the old toolmaker and tooling guy comes out to see the job and says "What the hell are you doing?"
Bob

BRIAN.T · Sep 14, 2020

This is excellent information. I appreciate your input. Tooling is tdb, I can certainly buy what I need for the job. I'll get some prices for cbn tomorrow. That will help for sure. The milled feature I can't use a face mill. It would be a 3/16 end mill, which incidentally is one of the plus or minus .002 features.

I've got almost 1000 parts to make. I think we can get it right towards the end of the run. Ha.

1953chevB · Sep 14, 2020

part is solid and no hollow areas? no small holes or center drills?

BRIAN.T · Sep 14, 2020

1953chevB said:
part is solid and no hollow areas? no small holes or center drills?

It's approx. 6" od 4" Id, 1/2 thick, with a 1/8" lip on the outter diameter. The ID has the milled feature, say two .180 diameter half holes.

The 1/8 lip would be the plus or minus .002, so I could likely rough, treat, grind the back side, then turn just the face, and mill the holes. most everything else is .020.

Mud · Sep 15, 2020

We make a 4140 part at 50-52, the ID is a taper with a keyway, the OD is ±.0002. we now turn both with CBN. At one time we used Cermets, but find the CBN lasts longer on the interrupted cut and is easier to hold size with. Sumitomo BN250.

EmGo · Sep 15, 2020

Grinding is nice. And accurate. And doesn't care how hard the material is ...

1953chevB · Sep 15, 2020

would be possible to rough out and then heat treat, leave .250 stock then finish it. inside diameters are tough.
even rough blanks can be distorted bad, but racking flat, or hang in a free state, and look into mar temper / mar quench it helps.
don't go crazy with feeds and speed, it will induce stress, and it will move.

Rick Finsta · Sep 16, 2020

For the milled feature can you use something like a SECO/Niagara 1/8" solid carbide high feed mill?

Mtndew · Sep 16, 2020

Phil in Montana said:
Harder than the hubs of hell

Not really. 50-55Rc is fine to machine. It starts to be a P.I.T.A. when the Rockwell gets to 60+.
When you're cutting 50+Rc turn the coolant off and use air blast. Obviously you'll have to slow down you speeds and feeds but once you dial it in it cuts rather easily.

Hardplates · Sep 16, 2020

Mtndew said:
Not really. 50-55Rc is fine to machine. It starts to be a P.I.T.A. when the Rockwell gets to 60+.
When you're cutting 50+Rc turn the coolant off and use air blast. Obviously you'll have to slow down you speeds and feeds but once you dial it in it cuts rather easily.

YES^^^

I routinely machine material in the 50 range with standard carbide tools. Small stepover, little slower SFM, no coolant (though I usually always run steel dry)

Personally I enjoy working with material in the 50sC and find you actually have to try to not get a mirror finish

EmGo · Sep 16, 2020

Hardplates said:
... you actually have to try to not get a mirror finish

Except for them damn feed marks ... now if you grind it ...

MattiJ · Sep 19, 2020

50 to 55 HRC is still machineable with "ordinary" end mills.

No experience of any of these but probably your next step if material is even harder:
Solid end mills for hardened steel - KYOCERA UNIMERCO
End Mills for Hardened Steels - Corner Radius - For Steels 45-68 Rc
YG-1 End Mills

This is were it starts to get expensive.. 1/8" YG1 nanograin carbide endmill is 40 USD and 2mm CBN endmill is 200 USD :eek:

snowshooze · Sep 19, 2020

Well, I started playing with hard 4140 and in the mill, I had to get used to low surface speeds and feeds. 50 SFPM and I haven't tried very heavy cuts.
IMCO tooling made for hard stuff.
Seems to work just fine.

Hardplates · Sep 19, 2020

snowshooze said:
Well, I started playing with hard 4140 and in the mill, I had to get used to low surface speeds and feeds. 50 SFPM and I haven't tried very heavy cuts.
IMCO tooling made for hard stuff.
Seems to work just fine.

50 SFM? Are you using HSS? Thats too slow even for tool steel in the 60s with carbide.

snowshooze · Sep 20, 2020

Hardplates said:
50 SFM? Are you using HSS? Thats too slow even for tool steel in the 60s with carbide.

Yeah, I mentioned I had to get used to it.

BRIAN.T · Sep 21, 2020

Fyi everyone, we ended up not getting the job anyway. I'm still following along, but the urgency has gone. Thanks for the knowledge.

Cutting 4140 heat treated to Rc 50-55

Cast Iron

Cast Iron

Cast Iron

Stainless

Diamond

Cast Iron

Cast Iron

Cast Iron

Diamond

Diamond

Cast Iron

Stainless

Diamond

Stainless

Diamond

Titanium

Stainless

Stainless

Stainless

Cast Iron

Similar threads