Announcement

Collapse
No announcement yet.

Cutting radius on shoulder on lathe

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts

  • Cutting radius on shoulder on lathe

    I need to cut a 1/8 inch radius between the shaft and shoulder for the flycutter I am making.

    Should I grind a tool bit with that radius or are there some calculations (and associated software) I can use to step the lathe around that radius?

    With either approach, how do I prevent from overcutting into the side that I didn't start on?

    It's not a high precision operation but I would like to learn the way that works for people. There will be other radii of various sizes to cut on the lathe in future projects.

    Thanks.

    - T

  • #2
    Originally posted by MinnesotaHSM
    I need to cut a 1/8 inch radius between the shaft and shoulder for the flycutter I am making.

    Should I grind a tool bit with that radius or are there some calculations (and associated software) I can use to step the lathe around that radius?

    With either approach, how do I prevent from overcutting into the side that I didn't start on?

    It's not a high precision operation but I would like to learn the way that works for people. There will be other radii of various sizes to cut on the lathe in future projects.

    Thanks.

    - T
    Grind a bit, or use an insert, like a TPG with the proper radius.

    As far as over cutting... can I assume that you left excess material there so that you don't have to undercut the shaft nor cut into the face. If you did, then you can (with the lathe off) touch off on the shaft and note your depth on the collars or set a stop. Then come out and touch off on the face, lock your carriage and note the reading on the compound, back off a whisker and then plunge it with the cross slide. It's basic and simple, certainly not perfectly precise, but will work quite well.

    Were I doing what you describe (for future considerations) I'd have ground a cutter with the proper clearances (or used an insert cutter with the right radius) and radius, used that for a finish pass on the shaft, then done a finish face (facing out from the shaft) once at the shoulder. Nice easy radius and clean transition.

    Quick dirty trick for pretty accurate measurements for facing is to use an indicator against your carriage on the headstock side of the lathe. Set indicator against carriage with cutter touched off on face, know how much deeper you need to take face cut. Make sure the indicator is set up for one full 360 degree sweep (.100 with a .001 indicator) then adjust dial (low) to zero with the extra depth of cut you need to make. So if you need to make a .010 face cut as a finish, then you touch off, and set indicator to 0 at one full sweep and then rotate back to 90. That way when you come into the cut you stop your power feed a little before the face, hand feed till the indicator zero's and then face out.

    With indicators make a habit of using a certain amount of pre loading I'll call it for lack of a better term... I try to always use one full sweep as a base then adjust from that. It eliminates having to count and possibly miscount on a spinning dial. This way I know that I can just watch the dial, kill power feed when the dial starts to move, and then manually continue to 0 and I'm done. No questions because I always set up the same way.
    Last edited by Walter; 10-23-2009, 02:46 PM.

    Comment


    • #3
      When I cut a radius at a shoulder I turn the shaft part to .010" oversize and at the shoulder I leave an area that is larger than the radius and I leave about .010" to take off the shoulder. Then I grind a 60deg V tool with the radius I want on the tip.

      I set the tool in the holder so it has the same clearance on each side of the shaft and shoulder. Then I blend the oversize area at the shoulder so the radius in there. Then I go to the end of the shaft and turn the shaft to size toward the shoulder and then turn the shoulder to the size from the shaft out to the OD of the shoulder.

      The trick is to be sure to leave enough material at the shoulder to make the full radius and after a few mistakes you'll learn how to do it.
      Last edited by Carld; 10-23-2009, 03:10 PM.
      It's only ink and paper

      Comment


      • #4
        The form tool methods described are the easiest way to make a radius, but be aware that the more tool edge in contact with the part, the greater the chance of chatter. More contact equals more cutting force required equals more power required. I don't know what kind of a lathe you have, but you may find that as you start your cut and the form tool starts to make a deeper cut, it starts to squeal or slows down your machine, or both. If that happens, you may have to create your radius with incremental cuts with a smaller radius tool. You can calculate the increments necessary with some simple trigonometry. If you start with cross feed (X), and your zero reference is the center of the desired radius, the relationship for a sharp tool (no radius) is longitudinal feed Z = SQRT((Radius^2)- (X^2)). Starting from zero-zero, infeed your X increment, then feed in your calculated Z value. Return to Z=zero and make another X increment, and feed to the new calculated Z. This works well until you get halfway around the arc, then you need to reverse the Z and X values in the equation and feed Z then X. You can tell when you are halfway when the Z value = X value. With a non-zero radius tool, the equation changes. If R = desired radius and r= tool radius, then Z=SQRT(((R-r)^2)-(X^2)) where your zero is the center of the tool tip radius. You need to adjust your feed increments to get a good approximation of the curve based on the tool radius. The bigger the tool radius, the larger the increment you can take, up to the limit of the machine to take a smooth cut. This also works for creating a radius on a part in a mill, just substitute Y for Z and use half your endmill diameter.
        Davis

        "Nothing is impossible for the man who doesn't have to do it himself"

        Comment

        Working...
        X