Speed and feed for countersink
Login to Your Account
Results 1 to 3 of 3
  1. #1
    Join Date
    May 2008
    Cumming, GA
    Post Thanks / Like
    Likes (Given)
    Likes (Received)

    Default Speed and feed for countersink

    Any advice for a HSS 1-flute 82-degree countersink in 1020? I'm looking to go .19" deep for 8-32 screws in .17" holes.

  2. #2
    Join Date
    Mar 2003
    Post Thanks / Like
    Likes (Given)
    Likes (Received)


    Yeah, something like 100 surface feet. If you're in a hurry, you can crank that up to oh, let's say 180, 250 if you have modern HSS like cobalt or micrograin.

    At that depth, you're going to cut a 1/2" circle with an 82 degree c'sink. half an inch = (.5 * pi) 1.571" circumferance. How many feet per minute?

    Let's calculate 100 surface feet. 100*12=1200, 1200 "surface inches".

    180 surface feet = 2160 "surface inches"

    250 surface feet = 3000 "surface inches"

    How many RPMs? Well, half an inch is 1.571" of circle, so just divide surface inches by circle circumferance.

    (100*12) = 1200. 1200 / 1.571 = 763.8 rpms

    (180*12) = 2160. 2160 / 1.571 = 1374.9 rpms

    (250*12) = 3000. 3000 / 1.571 = 1909.6 rpms

    Try 1000 rpms. 1000 * 1.571 = 1571 inches in a minute. 1571 / 12 = 130.9 feet per minute.

    130 fpm is probably a good speed for 1020.

    The feed for a single flute c'sink is probably comfortable around .001" per rev. You know where I'm going with this. .001 * 1000 = 1 inch per minute.

    How many revs? 190 to do the job, but if you start out at .100" above the stock in Z and feed down, a sharp point cutter will travel .3639". 364 revolutions of the tool at each c'sink. If your cutter is rotating at 1000 rpms, and there are 364 revolutions required, the math is easy. .364 of 60 seconds = 21.84 seconds.

    WOW! That's lots of time. A machinist would notice that immediately, and in embarassment, quickly ramp up the feedrate. Who the hell thought of 1 inch per minute?

    We quickly see the effects of the algorithm that produces dull tools and ugly surfaces. The factors in tool wear, listed in order of importance, are speed, feed, and depth of cut. The depth of cut, in this case, cannot be altered. Generally, depth of cut is "free". If the rigidity of the machine is adequate for increasing the width of a grooving or form tool, for example, you can remove more material at the same rates of feed and speed.

    Speed is the enemy, but feed is second-worst. If I really wanted my c'sink to last, and really needed my ass in gear, I would cut this somewhere around 1250 rpms and 2.5 inches per minute, and minimize the time spent cutting air.

  3. #3
    Join Date
    May 2011
    Central MA USA
    Post Thanks / Like
    Likes (Given)
    Likes (Received)


    Really??? Too much time on your hands? What is RPMS, revolutions per minutes?

    800 RPM 4.IPM .25 dwell, works perfect and i get about 500 pcs with a HSS bit. Carbide would last longer and take less time.


Posting Permissions

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