4140 44HRc Face Milling

Rick Finsta · Mar 19, 2020

I have always found 4140 annealed and pre-hard to LOVE SFM to get a good finish, both in turning and milling applications. I'm cutting material that has been hardened to 41-44HRc and not sure where to start. I'm using a Seco Turbo mill and their speeds and feeds seem crazy slow (I usually double them for 4140PH and that is my inclination here).

I also am not sure how to balance stepover and DOC on hard-ish material like this. I need to remove 0.106" and usually I will go as deep as 0.193" in material like this in a higher HP machine, but with around 10HP I am staying under 0.100". I also get a lot of smearing if I run a thin finish pass (say, 0.015" or so) in the 28-32HRc stuff so I was thinking of just splitting this into two even or near-even DOC passes with around a 6% stepover on a 2" face mill.

Thoughts? I've gotta get these knocked out and over to EDM for some holes. I don't wanna blow $300 on inserts testing things out. LOL

BSCustoms · Mar 20, 2020

Did a few hundred cubes of 4140 at 56hrc using some standard fair grade 5 flutes. Was running 100% axial with 10% radial, 700SFM and .009IPR. Dry with air blast. Had impressive tool life. Its very easy to get a nice finish in the low 40s rockwell.

Mtndew · Mar 20, 2020

41-44Rc isn't too bad, I'd probably just back off 10% on the RPM's and go from there.
And cut dry if at all possible.

ChipSplitter · Mar 20, 2020

For finishing, sometimes it helps to use coolant to prevent chip rubbing. It's worth a try at least, if you're struggling with surface finish.

D Nelson · Mar 20, 2020

I go about 70 percent step over and .05 depth works good for me
Don

Sent from my iPhone using Tapatalk Pro

Orange Vise · Mar 20, 2020

Trial and error is the name of the game when it comes to hardmilling with insert cutters.

Some ideas to try:

- Use a high-feed mill to rough out most of the material

- Roll your lead-ins and lead-outs with G02/G03

- Max your stepover. The normal 33%/66% sweet spot stepover doesn't apply because vibration is a more likely failure mode than rubbing. Vibration decreases at higher stepovers, i.e. 85-100%.

- If the workpiece is narrower than the cutter, position your toolpath on the centerline of the workpiece, not offset to one side

- You'll have to play around with axial depth of cut. The goal is find the maximum without burning up your cutter. Repeated passes at shallower cuts will wear out a smaller area of the insert. Cut too deep and you'll be fighting excessive heat and vibration.

- Determine SFM through chip color. Wherever you end up, it is what it is.

0.106" is a lot of material to remove. 4140 is relatively stable in heat treating, and normally I would leave more like 0.020"-0.030" total allowance for cleaning up both sides, but of course that depends on the size of the part.

Rick Finsta · Mar 20, 2020

Thanks for the replies!

There are some crazy tight calls on these parts, so roughing, then heat treating, then finishing would have been a PITA. After talking to folks around here and at the heat treater, I settled on pre-hardening and cutting it complete in that state. I'm planning on facing the material, EDM'ing the tight holes, then fixturing off them as data for all other operations using Mitee-Bite expanding mandrels and dowels. So I think I'm going to take it to finished width prior to EDM.

I have high feed mills for a lot of the work but the facing operation at finished hardness was something I wasn't originally anticipating having to do.

I'm most worried about tool life if I have to walk in the thickness at all. I know those inserts aren't going to like taking a tiny cut.

exkenna · Mar 20, 2020

"I have high feed mills for a lot of the work but the facing operation at finished hardness was something I wasn't originally anticipating having to do."

Feed mill inserts have a relatively heavy hone to withstand .030 to .040 feed per tooth. They have to survive in a wide range of materials, including nasty stuff like A36 with scale. Wouldn't last long with a sharp edge.
On a light DOC finishing pass the material can pile up on that blunt edge and smear or stick to the insert.
Tool life will suffer as well because you're basically burnishing the part and no heat is going out in the chip.
The heat will stay in the part and/or the insert. Could you rough with the feed mill and leave .015-.020 for the turbo mill using an insert with a sharp edge prep?

Matt_Maguire · Mar 20, 2020

At that strength condition any 4X40 is gonna stay put where you cut it. I like Don’s 70% dia step over. With 10hp unstable finish would be the only thing that would keep me from just taking the .016” DOC. I’d try it once on a chunk for sure.

Matt

Tichy · Mar 21, 2020

I had success recently with prehardened (Impax Supreme) using a Seco 40mm round insert face mill @ 2mm DoC and 15mm WoC airblast. Ran fine. Their high feed would probably be the better option, just made 100 cubes.

Rick Finsta · Mar 21, 2020

Well the machine has a maximum of 36 ft.-lbs. at 1500rpm... should I start at maximum torque and just see what happens? I usually like to run the 2" face mill at about 800-900rpm in alloy steels. 1018 or 1020 she seems fine up around 1200-1500rpm with these inserts but never tried it with a 4XXX series.

Tichy · Mar 21, 2020

900rpm sounds very low. High speed low feed is your friend with alloy steels, I think, especially with a low-HP machine?

Rick Finsta · Mar 21, 2020

I often have to cut with coolant since I don't have air blast but for face milling I will be fine and can likely kick the RPM up. So I tend to keep the SFM low to keep the heat down. That said, I will probably start at 1200rpm and about 0.004ipt at 0.06" DOC and split the face in two with the WOC as best as I can. If the chips look good I'll stay there, if they need less or more SFM I'll adjust accordingly.

Rick Finsta · Mar 21, 2020

1200rpm (630SFM) was waaaay too fast. Spark show. Running 570-600rpm and 0.004ipt is working well at about 0.05" DOC, but I'm getting a ca. 0.001" step without taking a finish cut. I'll try breaking it down into a single large cut and a 0.015-0.025" finish cut. I can also try cutting at 90deg and see if that works since it will even out the stepover. I'll also try a few other things to get the toolpath closer to 50/50 across the face. Yes, I could finger-CAM it but that isn't how I work LOL.

Search

Largest Manufacturing Technology Community on the Web

Search

4140 44HRc Face Milling

Rick Finsta

Stainless

BSCustoms

Cast Iron

Mtndew

Diamond

ChipSplitter

Titanium

D Nelson

Stainless

Orange Vise

Titanium

Rick Finsta

Stainless

exkenna

Stainless

Matt_Maguire

Stainless

Tichy

Aluminum

Rick Finsta

Stainless

Tichy

Aluminum

Rick Finsta

Stainless

Rick Finsta

Stainless

Similar threads