Announcement

Collapse
No announcement yet.

Pocketing with an End Mill

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

  • Pocketing with an End Mill

    I have been asked to give some thought as to how to proceed to
    cut a 1.5" x 5.0" rectangular pocket 0.550" deep in leaded steel
    using a 1/2" HSS end mill with coolant on a sturdy vertical mill.

    Wouldn't the primary approach be to make a series of roughing passes
    in a spiral pattern, leaving about 0.020 along each wall and increasing
    depth by 0.165". Then take a final pass finishing the walls and bottom
    to tolerance?

    .

  • #2
    Pocketing

    Is this on a manual or CNC mill? How many pockets?
    Last edited by Toolguy; 11-17-2010, 07:08 PM.
    Kansas City area

    Comment


    • #3
      A powered manual mill.

      Just one pocket.

      .

      Comment


      • #4
        I'd drill a hole in each corner to mark the limits of your travel, then plunge into one of them with a roughing cutter. Dig out most of the meat, then come in and finish with a regular end mill.

        Given only the finishing end mill, I'd start with a slot going down the center of the pocket-to-be. Then I'd 'spiral' my way out to the finished size keeping the cutter maybe half engaged at all times. Finish pass somewhat lighter.

        Comment


        • #5
          If u want to maximize end mill life:
          Rough out most of the material by using a 1/2 stub drill to make a pattern of holes.
          Use high depth of cut (e.g. 0.5 deep) and low width of cut (1/8" sideways).
          Climb cut if your mill doesn't have much backlash.

          Comment


          • #6
            Remove most of the material by drilling first.
            Use the largest drill possible.
            Then use the endmill to hog out the remaining material, stepping over each pass in a rectangular pattern.

            Comment


            • #7
              Being an Amateur HSM, I would start with a 5/8 drill about 0.4 deep near a corner. Then cut the pocket to full depth to .020 shy of the edges in two depth passes. Finish to dimension with a climb cut. I run a Bjur clone with Rustlick water soluable cutting fluid and vacuum the swarf. I prefer the good sharp carbide mills that followed me home from an auction but HSS will work fine.
              Byron Boucher
              Burnet, TX

              Comment


              • #8
                Some additional considerations - the machine has a DRO and backlash
                compensation.

                RK, if your method involves plunging a 0.500 EM to near finished depth
                (0.550") and then moving laterally, I imagine there might be trouble.

                The rule of thumb I learned was to take a cut of no more than 1/2 the
                diameter of an endmill, preferably a good deal less than this. I proposed
                a conservative 0.165" because of the amount of the large amount of the
                cutter that was going to be engaged.

                I see that beanbag is suggesting 0.500" depth, too.

                .

                Comment


                • #9
                  Boucher - a parameter is the limitation of using only a 0.500 HSS end mill.

                  .

                  Comment


                  • #10
                    EddyCurr,

                    I think you nailed it in your first post.

                    Personally I would leave more than .020" on the sides when roughing, its all too easy to use that much up when roughing. It just means you would finish the sides in say two passes, rather than one.

                    I would use a two-flute slot milling cutter, so you can plunge and mill. No need to try and use too much depth of cut, try your .165" and see how it goes....If you want to speed things up, a roughing cutter allows you to take a depth of cut the same as the cutter diameter, though even then you have to be careful that the endmill isn't being dragged out of the collet.....

                    Forget about drilling holes and climb milling IMO !
                    Last edited by Peter S; 11-17-2010, 07:53 PM.

                    Comment


                    • #11
                      Originally posted by EddyCurr

                      The rule of thumb I learned was to take a cut of no more than 1/2 the
                      diameter of an endmill, preferably a good deal less than this. I proposed
                      a conservative 0.165" because of the amount of the large amount of the
                      cutter that was going to be engaged.

                      .
                      A slightly more sophisticated rule of thumb is based on the cross sectional area of cut, i.e. DOC x WOC. This is approximately representative of cutting force. So depending on rigidity of machine and endmill material, I might say something like diameter squared for Aluminum (1/2x1/2), and maybe half that for steel (1/8 square inches total).

                      Next, I would say maximize DOC because that puts more flute into the cut and thus stabilizes the cut, or reduces vibrations. It also wears the end mill more evenly.

                      Finally, I like to take lighter widths of cut (glancing passes) because the flutes make a more gentle entry. You can increase the feed rate over what is normally calculated due to chip thinning effects.

                      Comment


                      • #12
                        如果寄件者要求您在 以外完成交易,請勿回覆對方,因為這是違反
                        政策規定的行為,不但可能有欺詐意圖,這類交易也不能享有買家購物安全保障。進一步詳情請到:

                        Comment


                        • #13
                          Originally posted by beanbag
                          If u want to maximize end mill life:
                          Rough out most of the material by using a 1/2 stub drill to make a pattern of holes
                          This was the technique I first used when pocketing, but I seemed to wear my cutters more quickly this way, I put it down to the effects of constantly moving form air to metal to air.

                          Nowadays I drill one central entry hole and spiral out from there.

                          Not claiming any depth of knowledge here, just one amateur's experience.

                          Comment


                          • #14
                            Eddycurr
                            You have it exactly right...dead nuts....Bob too

                            On Steel, no more than 1/3 the diameter for DOC (.5/3=.166 ")
                            Fastest path is a spiral ( rectangular spiral in your case) so you spend no time cutting air.
                            Finish pass is required, and is really based on feed rate.
                            Higher feed rates yield greater deflection which requires larger finish pass allowances

                            Rich
                            Drilling holes in the corners is nice, but takes longer as it requires 2 setups
                            Green Bay, WI

                            Comment


                            • #15
                              Originally posted by EddyCurr
                              RK, if your method involves plunging a 0.500 EM to near finished depth (0.550")...
                              Roughing cutter. Key word there, and you're plunging into a drilled out hole.

                              Also, I would rough as close to full depth as I could if for no other reason than to distribute the wear on the whole flute rather then just the first 1/8 inch over and over. I've done it at least as many times as I have thumbs and it's worked nicely at least once. You're cutting leaded steel? EVEN BETTER!

                              But the original post says that you just have a single end mill. No drills, no roughing cutter, just an end mill. So none of the above applies.

                              Comment

                              Working...
                              X