Page 1 of 7 123 ... LastLast
Results 1 to 10 of 61

Thread: Reaming Hardened Steel

  1. #1
    Join Date
    Jul 2017
    Location
    Springfield Mo
    Posts
    605

    Default Reaming Hardened Steel

    Bit of an issue, im working on a butterfly knife design, and said design has the blade running on a bushing that sits in a 3/16 hole in the blade. Ive been drilling and reaming these before heat treatment, but after all is said and done the bloody things have opened up by about .004", as well as being slightly ovate. My question is, is there any sane way to ream these holes out after heat treatment, with the steel sitting at about 61rhc? The present best idea ive got is to drill the holes to .182" or thereabouts before heat treatment, then go back to the mill afterwards and finish off those holes with a carbide tipped 3/16" reamer.

    Am i insane for thinking this would work? Can i reasonably expect carbide to cut through material at that hardness, or will i just smoke a reamer?

  2. #2
    Join Date
    May 2011
    Posts
    870

    Default

    I think the reamer idea would work provided you run it slow, but given that you have that "slightly ovate" hole after hardening you might still have some problems.

    Another idea might be to use a 3/16 carbide end mill with a very slow upfeed on the mill knee rather than using the quill. I think you can control the upfeed on the knee, even by hand, easier than the quill. If I HAD to use the quill I'd put a bit of tension on it by tightening the quill lock a little. On a hard irregular shaped hole the reamer/mill cutter would have a tendency to bounce when it engages the workpiece or it could chip the carbide. By having a very rigid set up like this there is abetter chance of getting good size and a round hole.

  3. #3
    Join Date
    Dec 2016
    Location
    Helsinki, Finland, Europe
    Posts
    3,597

    Default

    Carbide reamers are quite pricey to lea(r)n on.
    Since the hole is so short you could grind it with small diamond stone and toolpost grinder in a lathe. Or maybe even bore with small carbide boring bar but getting the hole round and to correct size by boring can be tricky at 61hrc

  4. #4
    Join Date
    Aug 2009
    Posts
    6,553

    Default

    I would try the carbide reamer. I would also cut the shank as close to the reamer flutes as you can leaving just enough to chuck up in the collet. This will eliminate any deflection from the shank.

    JL............

  5. #5
    Join Date
    Oct 2014
    Posts
    468

    Default

    There are carbide drills advertised as being able to handle low 60 rc. You need a rigid setup (milling machine) and a lot of nerve to feed the drill into a hard piece of steel but it works. I would think a carbide endmill would work too.

  6. #6
    Join Date
    Feb 2012
    Location
    Metcalfe, Ontario, Canada
    Posts
    1,375

    Default

    Do you really need the pivot area that hard? Seems to me that would be pretty brittle and it annoys the hell out of me to break a blade off at the end I don't even cut with.

    I don't know anything about fancy knife steels, though, maybe it can't be softened locally.

  7. #7
    Join Date
    Mar 2005
    Location
    Toronto
    Posts
    11,111

    Default

    A carbide reamer might work, but its an expensive experiment if not. One should expect tool steel to move a bit on heat treating and you usually deal with it afterwards by grinding .......or in the case of small holes, lapping. The laps don't necessarily have to be adjustable, just a piece of brass that is a tight fit with some medium compound on it can do the trick.
    .

  8. #8
    Join Date
    Jan 2008
    Location
    Traverse City, MI
    Posts
    1,603

    Default

    Quote Originally Posted by Mcgyver View Post
    One should expect tool steel to move a bit on heat treating...
    That fact can spell doom to a carbide reamer they don't follow a hole like a HSS reamer will and any deflection will snap them. Whenever I used a reamer in hardened steel I would plunge an undersized (reground) carbide cutter through first to re-establish the hole location.

    In your case, I would be tempted to just try plunging with an end mill. Note that unless your mill is very rigid, it will likely cut a little oversize.
    George

  9. #9
    Join Date
    Mar 2015
    Posts
    3,908

    Default

    My thought is if you're doing many of these, as your own product, to change the method of heat treat. As others said, does the entire blade shank need to be hardened? I don't make knifes, I don't know.

    Sent from my SM-G950U1 using Tapatalk

  10. #10
    Join Date
    Jan 2010
    Location
    Kansas City area
    Posts
    5,694

    Default

    When making precision dowel pin holes in hardened die blocks, we always drilled and reamed them enough undersize before heat treat, then lapped out the last thou. after. If you use an air hardening tool steel like D2 or S7 (my preference), the steel doesn't move as much during quenching. This is because air quenching is cooling much more slowly than liquid quenching. It all expands when heated, cooling slowly gives it more of a chance to go back closer to where it started out before it solidifies. You don't say what alloy you're using.

    As for reaming the hole after heat treat, I agree with those that said the tang/hinge area could be drawn back some. Even at 50Rc for the tang, the blade would still be very strong. I would still want the cutting edge to be 58 - 60 or so to hold an edge. At 61Rc you're going to go through a lot of carbide reamers. I would use a carbide spade drill for that, they are way cheaper and tougher. Run any of them dry. If you use cutting oil, the carbide will just skate off the steel till you get enough pressure to rupture the carbide. If dry, it will bite in right away.

Posting Permissions

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