What's new
What's new

Need to mill key slot in hardened shaft - how?

clomb

Cast Iron
Joined
Feb 1, 2010
Location
Newberg, Oregon
I need to mill a 1/2" key slot in a 2" hardened splined shaft. Will carbide cut through the hardened shaft?

Thanks in advance,
Chuck
 
Quick rule of thumb;-

If you can mark / cut in to it with a fine file, it can be machined - in many cases with HSS**,......... carbide is better but you need a very rigid machine or it will chip cutters like they're going out of style.

** Cutting speed of 20 - 30ft / min and as rigid as possible.
 
Chuck,

I wonder why a shaft with splines would need a key installed?:confused:


Stuart

Stuart,

I just pulled a broken axle shaft out of a john deere commercial mower.

Spline end in the differential. Keyway on wheel hub end.

Big B
 
Last edited:
It may be possible to mill, but I'd want to use a cnc for it, reason being that I would program the cut as a long continuous ramp with a descent rate of about .010" per orbit of the slot, using a bullnose endmill...something like 1/4" diameter (TiAlN coated) with .015"r flute tips. Run the tool at about 300 sfm and 40 ipm for a start and see how it goes. Air blow the chips away.
 
I had a very similar job a year or two back. Hardened steel shaft, splined on one end, keyed on the other. It was for a "bobcat" (or something.) The key way was bashed out from being too loose (or something.) Not only was the shaft hardened originally but was now also work hardened on top of that.

I got a couple of 3/8" carbide endmills. I forget which brand and coating but I can check later. I mounted the shaft as solidly as I could between big V-blocks on my Rockwell vertical mill. It was mounted so the new slot would be cut 180* away from the old one.

I forget the spindle RPM but probably in the 600RPM range.

I came in from the side, about 0.050 DOC, feeding slowly in Y until I was on center, then fed in X. As HFD says I could not feed in Z unless I was also feeding in X (ramping.) I cut dry and no air. Weird orange burning chips that seemed to move in slow motion. I cut a 2" long slot about 3/8" deep. Using air to clear the chips would have been good (or cut horizontally) because I damaged the cutter by re-cutting chips. Got the job done though. Cost of trashed cutter about $20.

ETA: The milling cutter I used was an ATRAX brand 3/8" 3/8 shank 4 flute solid carbide part no. 85332245.

-DU-
 
Last edited:
Maybe the shaft is case hardened. If you can take a 1pass to cut under the hard layer the endmill will last longer. If you try to machine it with multiple thin cut on the end of the endmill you have more chance to dull it. You can also plunge rough the slot before finishing.
 
Lots of good input.

This shaft is from a hydraulic gear box. The shaft was originally driven using an internal spline. The customer is converting the unit to be driven via an L-Coupler that slips over the shaft. The coupler is keyed and so now the shaft must be keyed.

Chuck
 
The whole point of hardening stuff is so that it can't be cut, doh!

You may as well anneal it and and re-harden it after cutting the keyway. If you go ahead and cut the keyway with kryptonite or whatever it will get so hot it will be annealed anyway so you may as well do it in a controlled fashion.
 
The whole point of hardening stuff is so that it can't be cut, doh!

You may as well anneal it and and re-harden it after cutting the keyway. If you go ahead and cut the keyway with kryptonite or whatever it will get so hot it will be annealed anyway so you may as well do it in a controlled fashion.

If only that were true, it would be a useful feature for drilling out broken taps.

Hard milling does not generate a heat affected zone. But you need light cuts with firm continuous feed and pressure to make the tool last for the duration. Annealing and rehardening a shaft is a major endeavor by comparison, what with decarb and warpage going on, plus the uncertainty of what you get when you reharden it.
 
I key 54 Rc shafts all the time with carbide. You just aren't going to cut deep in a single pass. Keep it shallow, lots of passes, it will take some RPM. Make sure you carbide doesn't thermal shock so you can run coolant.
 
I just had to cut some 10mm x 5mm deep blind keyways in 6 Thomson case hard shafts,above 60 Rc.I pre drilled with a carbide drill to depth then plunged and milled with an OSG Exocarb end mill.They are advertised to cut 70Rc,however MSC cost was over $100.00 for the mill,which I managed to destroy by recutting chips.I was going to post and ask I anyone had any better ideas or better tool sugestions.I had tried an Atrax uncoated endmill but it dulled right away.
Randy
 
For keying a thompson shaft you can scribe the key on the shaft and with a angle grinder grind carefully the first ~.060''. Those shaft are case hardened. Then you can mill the slot with carb endmill. I have machined some cylinder rod for a job. The chrome layer is the hardest to get by... then the hard layer is not that hard for a carbide endmill just don't crank speed and feed, the rest is soft. I'll use regular quality (read price) like fullerton end mill. Those hard milling application are not optimal to use extra quality end mill (rigidity, full slotting and constant hardness variation).
 
I just had to cut some 10mm x 5mm deep blind keyways in 6 Thomson case hard shafts,above 60 Rc.I pre drilled with a carbide drill to depth then plunged and milled with an OSG Exocarb end mill.They are advertised to cut 70Rc,however MSC cost was over $100.00 for the mill,which I managed to destroy by recutting chips.I was going to post and ask I anyone had any better ideas or better tool sugestions.I had tried an Atrax uncoated endmill but it dulled right away.
Randy

You cannot approach milling hardened steels with monster cuts. While carbide is hard enough to cut hardened steel, it must be forced to cut. This means a positive feed and decent chipload is required with every chip. But the stiffness of carbide, while better than HSS, is not infinitely stiff, and taking a deep cut in hard steel simply requires more tool pressure than the tool shank can deliver. On a light cut, you can force the tool under the surface and it will deliver a chip, but you need to minimize any and all dwell periods with the tool engaged in the work.

I would recommend a bullnose grind (radius corner tips) on any tool that is expected to live through a hard milling session. You're going to lose the razor sharp pointy corners anyway, and then that will make further progress difficult, because they most often dull and create the effect of a heavily honed negative rake tool.
 
Chuck,

This may not apply to your situation, but I have annealed the ends of hardened ballscrews to machine a feature on them or turn them to size.

This annealing only affects the area heated and doesn't ipact the strength of the ballscrew. This is common field practice and I believe the ballscrew assemblies even came with a small directive on the procedure to accomplish this.

Maybe these are only case hardened...maybe your shaft is a through hardened item..I don't know if this would make a difference.

Stuart
 
Spot annealing a shaft is surely going to bend it (for a keyway milling application). Even hard milling may cause an undesirable stress relief which could cause some runout, but you'd have to check the part after it is done to determine the extent of it. If you were to anneal it in a rotary fashion (heat a zone on the shaft whilst spinning it in the lathe), perhaps it will be okay.
 
Depends on the hardness but generally, your axial depth of cut is going to be ~2% of the tool diameter for full diameter width cuts. A good quality 3/8" end mill, designed specifically for 40+ HRC machining, will work fine at 320-260 sfm (45-55 HRC respectively). Chip load will be somewhere in the .0015-.002 inch/tooth range.

You'd have a much easier time using a hi-feed end mill to rough the slot; something like a Mitsubishi HFRB-series, or of course trochoidal is an option if you have the capabilities. Then finish the walls with a good 6-flute.

Lots of ways to skin that cat but the 'hi-feed' mill has very strong cutting geometry... thus, great tool life in these materials.

Chuck
 








 
Back
Top