Tool to mill flats behind a shoulder, c-axis mill turn, using polar

I have a part that needs wrench flats, the flats are behind a turned diameter, maybe .093" deep, so I can't use polar and an end mill to reach them. My machine is a vanilla c-axis mill turn, no Y. I have considered options like mounting a Woodruff key cutter in an er25 and reaching past the shoulder, the reach would be 2-3/8", but that seems like a recipe for a lot of chatter, and slow. I am using all my straight (x-axis) live tool holders to drill and tap other holes, between the turning and milling I've got room for one angled live tool holder(z-axis). My parts are annealed 4140, and I am setting up a few hundred of them. I have a real nice tool guy, he recommended a $1200.00 insert slotting mill, eight 3mm wide passes for each flat,
I am real sure someone out here has a much better solution for this than a woodruff cutter or a $1200.00 slot mill. This is sketch is not to any scale.

Solid carbide endmill with the proper neck clearance ground. We used to by varimills and pay about $15 to a local grinder to grind it into a woodruff cutter of sorts. Only need about .200 on the diameter removed.

Agree with lx545, pretty easy to create the relief you need with a spin indexer on a surface grinder. With that stickout I'd be wanting a 5/8 or 3/4 endmill. Give it some relief on the back edges by angling/tilting the spin indexer and it will create a better finish on the back side shoulder.

Grinding an endmll is very promising, nobody local to do that for me though. I was thrashing around MSC and found a Seco slotting mill,
1.5 Inch Cutter Diameter, .375 Inch Cutter 9133412 - MSC has anyone used one of these in an application where it isn't in a balanced cut?

endmill is easy to ship - a couple of folks on this forum could surely do such a thing
helical/harvey has some relieved endmills, maybe not enough though

That disc mill will work flawless. Used several to mill sledrunner keyways in shafts. May have to play with conventional vs climb mill to make it easier on the machine. I've always conventional milled in a live tooling lathe unless finish is a problem because it seems easier on the machine.

Perfect Y axis application, if you had it. Might be a candidate for polygon turning, if available on your machine. If it's capable but you didn't buy it initially, it's usually just a software switch that can be added.

Modifying a 5/8" or 3/4" End Mill would definitely work for the application but if you don't have time to modify a tool then I have had good luck with the Carmex CMT System for Long Reach Groove Milling and Threading. They would have the Reach you need in a Steel Coolant Thru Body or a Carbide Coolant Thru Body, here are links to each:
CMT Groove Milling Inserts
CMT Steel Long Reach Coolant Thru Holder
CMT Carbide Long Reach Coolant Thru Holder

The Insert combined with the Steel Holder would give you an offset of .145" per side and the Insert combined with the Carbide Holder would give you an offset of .1775" per side so it would give you the milling depth you need. Each also has the Reach and the inserts would be a .240" Width (the only thing about the inserts is they do have a .008" Radius, not sure if that is acceptable or not). In 4140 run it at 300 SFM and .004" CLPT.

If it's short run and you are ok with just modifying the neck of a tool then a Push/Pull Cutter is nice. They have a 3/4" Head Diameter x .250" Width x .375" Neck Diameter x 3/4" Neck Length x 4" OAL x 4 Flute ALTIN Coated Cutter that you'd just need to neck back to the 2-3/8" you need:
Push/Pull Cutter

Hopefully this helps!

Mike