Page 1 of 2 12 LastLast
Results 1 to 20 of 38
Like Tree1Likes

Thread: Need to mill key slot in hardened shaft - how?

  1. #1
    clomb's Avatar
    clomb is offline Cast Iron
    Join Date
    Feb 2010
    Location
    Newberg, Oregon
    Posts
    278

    Default Need to mill key slot in hardened shaft - how?

    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

  2. #2
    magicmaker is online now Hot Rolled
    Join Date
    Oct 2006
    Location
    Tucson, AZ
    Posts
    534

    Default

    I'd grind the slot on my surface grinder.
    Jim

  3. #3
    Limy Sami is offline Diamond
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    11,718

    Default

    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.
    S_W_Bausch likes this.

  4. #4
    clomb's Avatar
    clomb is offline Cast Iron
    Join Date
    Feb 2010
    Location
    Newberg, Oregon
    Posts
    278

    Default

    Thanks.

    Unfortunately no surface grinder.

    Chuck

  5. #5
    atomarc is online now Titanium
    Join Date
    Mar 2009
    Location
    Eureka, CA
    Posts
    2,061

    Default

    Chuck,

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


    Stuart

  6. #6
    Big B is offline Stainless
    Join Date
    Jun 2009
    Location
    Michigan, USA
    Posts
    1,063

    Default

    Quote Originally Posted by atomarc View Post
    Chuck,

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


    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 by Big B; 04-19-2011 at 08:35 AM. Reason: Spelling

  7. #7
    HuFlungDung is offline Diamond
    Join Date
    Jan 2005
    Location
    Canada
    Posts
    6,622

    Default

    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.

  8. #8
    David Utidjian's Avatar
    David Utidjian is offline Titanium
    Join Date
    Jun 2006
    Location
    Mahwah, NJ
    Posts
    3,041

    Default

    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 by David Utidjian; 04-19-2011 at 10:12 PM. Reason: added stuff about cutter

  9. #9
    altered is offline Aluminum
    Join Date
    Apr 2007
    Location
    Qc, Canada
    Posts
    113

    Default

    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.

  10. #10
    clomb's Avatar
    clomb is offline Cast Iron
    Join Date
    Feb 2010
    Location
    Newberg, Oregon
    Posts
    278

    Default

    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

  11. #11
    jscpm's Avatar
    jscpm is offline Hot Rolled
    Join Date
    May 2010
    Location
    Cambridge, MA
    Posts
    689

    Default

    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.

  12. #12
    HuFlungDung is offline Diamond
    Join Date
    Jan 2005
    Location
    Canada
    Posts
    6,622

    Default

    Quote Originally Posted by jscpm View Post
    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.

  13. #13
    garandguy's Avatar
    garandguy is offline Plastic
    Join Date
    Jan 2010
    Location
    Hard Desert of Utah
    Posts
    16

    Default

    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.

  14. #14
    Abom79's Avatar
    Abom79 is offline Stainless
    Join Date
    Feb 2011
    Location
    Pensacola, FL
    Posts
    1,269

    Default

    If your able to use flood coolant, get a couple good carbide endmills and shouldnt have any problems.

  15. #15
    ratbldr427 is offline Cast Iron
    Join Date
    Mar 2006
    Location
    jacksonville,fl.
    Posts
    452

    Default

    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

  16. #16
    altered is offline Aluminum
    Join Date
    Apr 2007
    Location
    Qc, Canada
    Posts
    113

    Default

    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).

  17. #17
    HuFlungDung is offline Diamond
    Join Date
    Jan 2005
    Location
    Canada
    Posts
    6,622

    Default

    Quote Originally Posted by ratbldr427 View Post
    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.

  18. #18
    atomarc is online now Titanium
    Join Date
    Mar 2009
    Location
    Eureka, CA
    Posts
    2,061

    Default

    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

  19. #19
    HuFlungDung is offline Diamond
    Join Date
    Jan 2005
    Location
    Canada
    Posts
    6,622

    Default

    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.

  20. #20
    cmailco's Avatar
    cmailco is offline Hot Rolled
    Join Date
    Aug 2010
    Location
    Dallas, TX
    Posts
    949

    Default

    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

Page 1 of 2 12 LastLast

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •