What's new
What's new

Cutting 4140 heat treated to Rc 50-55

WoW! seriously surprised by the ceramic and cbn mentions. Pretty much cut up to 58Rc a2 and D2 with coated carbides "back in the day", sure the grinds and coating and carbide is soooo much better now. Production, dunno, was job shop work, maybe different for 1000 pieces.... I will say back then 4140 heat treated was a nightmare for size and stability, was cheaper to use more expensive a2 for heat treat stability...
Heat Treating 4XXX series alloy at these elevated levels is asking for a fracture, your heat treater should know better. 48 max, you need to go to tool steel if you want material this hard.
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.

Not that it matters anymore, but I hope that 50SFPM is a typo. I cut hard mold steels S-7, H-13, all in the mid to upper 50's R.C. and do it all day in the 450-550 SFPM range for rouging, and much higher for finishing.
I understand that the OP did not win the job, but in the interest of posterity, I'm going to post anyway.

Turning 50+ 4140 should be no problem.

Leave around .010"-.020" stock for finish-turn. CBN would be my first choice.

Sumitomo rules the CBN world, although that depends on the rep you get. If the individual rep doesn't know CBN turning well, move on. I worked for Seco, and know their lineup pretty well. While everyone in the industry wants to give the automatic nod to Sumitomo, I can say at least that Seco has a nice product lineup for CBN turning - and this part is critical - they have a lot of resources for the sales-person, and therefore the customer to take advantage of in regards to education & application. CBN060k would be my starting grade. Probably start running dry - maybe move to wet cutting if it made sense.

If you don't want to use CBN, Seco TH1000 carbide grade will do the job quite well. In fact, this grade works so well in so many applications, that every shop should have a pack of CNMG432W-MF5 TH1000 laying around for the odd hard-turning job. I could go on more & more for how much I love this grade. We've used it in production turning for over 5 years, and nothing has displaced it yet. But I digress...

For your 50hrc turning, again, leave .010-.020" on the diameter for finish-turning. Start around 250sfm, with coolant, feeding .006-.012"/rev, or as your finish requirements dictate. You could probably increase speed up to say, 350sfm if things were behaving well.

For milling in the 50's, look for endmills with big corner radii, high-feed geometry where you can for end/face cutting. In the past anyway, the consensus was to look for coatings with lots of aluminum, as the Al was supposed to turn into aluminum-oxide at high temperatures? I honestly can't keep up today as I don't do much milling anymore. I will say though, that Seco had a deep bench in regards to hard-milling. Between the Niagara & Jabro lineups, I'm sure they have a dizzying array of hard-milling products by now. They also have some incredibly smart, well experienced guys on the payroll to help with hard milling applications too, so I would feel confident that they could get you going well in short order.
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.

Just off the top of my head.....using a 6 flute YG1 endmill (if 6 flute is available for the diameter you need) I would be around 450-600 SFM, 45-60 IPM, radial DOC .05 x tool dia. , axial DOC 1-1.5 x tool diameter. Air blast. Good toolholders are a must....avoid spring collets.....think milling chucks, shrink fit, hydraulic holders etc.
Generally when milling hard(er) material you should not see a bunch of sparks flying around.....the one exception i have ran into is 4140....sometimes you will see a few sparks even when its working correctly.
I have succesfully used these parameters for the last 15 years......btw.....50-55rc barely qualifies as hardmilling :)
Hardmilling starts to suck at 65+ Rc....parameters change.
Rycut 40

Don't do this. Leave minimal.

Back in the 1960's a young engineer(me)worked for a pump company in their rotary (oil) pump department. Some pumps for abrasive/dirty liquids were made with a hardened steel shaft option. Those shafts were solid stepped diameters in the range of 1 to 3 inches depending on the size of the pumps and slotted for square keys. There were no internal diameters other than center holes. Spec was 4140 at 50-55 Rc. The best machinist in the shop had a Monarch EE and did the rough turning before heat treat. Finish all over was conventional grinding on centers. Key ways for impeller gears and couplings (to drive motors) were sized before heat treat; but might well have gotten some further attention after the grinding. The material used was a proprietary leaded 4140 product from Ryerson they branded as "Rycut 40". Referred to today as 41L40.
For the milled feature can you use something like a SECO/Niagara 1/8" solid carbide high feed mill?

I use the Niagara stabilizers w/ .02 or .03 corner breaks when milling our hard materials. I use MA ford hi-roc for drilling hard surfaces.