Announcement

Collapse
No announcement yet.

Bridgeport plunges a larger diameter than it slots...

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

  • Bridgeport plunges a larger diameter than it slots...

    The title says it all. I used a 3/8 endmill to plunge holes for a short slot. When I went back to clean up the slot the sides were not smooth...little dips from where the endmill plunged a larger diameter. This is consistent and on both sides of the slots. Is this abnormal? I don't remember ever having this issue before and I've slotted with the same technique.

  • #2
    The endmill probably grabbed the sides of the hole a little and orbited a bigger hole. Endmills are bendy! If you profile the exterior outline of a shape (say a rectangle on a non-CNC mill) with a heavy cut, and do the same thing but divide the job into several lighter cuts, your shapes will mic to different sizes, by a surprising amount, even on a rigid machine.

    Comment


    • #3
      Yes, it is abnormal in that you probably didn't want it to happen, but as rklopp says it will happen usually every time that you plunge an end mill.

      Because there is essentially no point on an end mill, whichever flute happens to be cutting at any moment presents an unbalanced cutting force which will push or pull any deflection, backlash or looseness all in one direction from centerline.

      It is one of the reasons that drills have points rather than flat ends.

      Dave

      Comment


      • #4
        Here's the rule: never use an on-sized end mill to cut a close tolerance slot or a key seat.

        Everything is made out of rubber. Everything, even the stiffest most massive machine tool deflects under load sometimes to a surprizing degree. A typical small shop turret mill is not a monument to structural rigidity. This can be simply demonstrated by plunging an endmill into the work without first drilling an undersized hole. A center-cutting endmill because it's flat has no self-centering cutting geometry. Even the best center cutting endmill in a turret mill spindle plunging into solid material will wobble visiblely to the naked eye.

        The cutting forces deflect the cutter to the side. The cutting force varys with the chipload thus the cutter deflects more or less in proportion to the feed rate. The deflecton is not small; it may amount to 0.012" for an ordinary 3/8" endmll cutting mild steel 3/8" deep.

        The most reliable way to cut an accurately sized slot is to use a 1/32" or more undersized endmill to rough out the bulk of the material. Then offset 1/2 the desired slot width minus the cutter size and take a finish pass on each side of the slot. In elongated bolt holes used to adjust a motor on its baseplate to tension a V belt some error will not matter. If fit is important as in a keyseat or other close tolerance feature care should be taken to ensure the slot width is correct.

        There are those who assert you can cut an accurate slot in a single pass with an on-size endmill cutter but they are mistaken. I can only suggest they never check their work.
        Last edited by Forrest Addy; 03-17-2010, 03:11 AM.

        Comment


        • #5
          Same thing happens with drills - that's why they make reamers. Perhaps if you had a zero run out mill with an absolutely immobile table and an end mill that was manufactured with zero imperfections regarding symmetry then you may plunge the perfect hole - well, no, that means the work has to be as perfect as your machinery. Not going to happen - use a smaller end mill and machine to spec.

          Comment


          • #6
            HSS End mills will walk, especially the smaller ones. Carbide is much better, but as the last poster said, they can pull the backlash out of the table. If the slot is to be a through slot, such as a flat plate, drill the ends through a size or two smaller then run your end mill through to make the slot,, however they will still usually walk to one side. If you need a slot on size, use an under size end mill and step over to clean up to size. Whenever making a keyway (blind on one end or both) I always use a reground end mill or one size smaller endmill, for that reason. start on the center line of the shaft and step over half the difference on both sides.

            Comment


            • #7
              S-l--o---w----l-----y

              The ideal machine for cutting gears, splines, slots and key-ways (where it suits) is a horizontal mill using a good sharp side and face cutter or profile/d cutter to suit. Or use a slotting or side and face cutter on a milling arbor on a vertical mill:




              With an end mill I prefer to drill the ends to be the same as the slot is to be and use a short 2-toothed slotting end milling cutter to less than full depth and the end milling cutter one size under the width of the slot.

              I finish off with a normal end-milling cutter.

              I don't give a big rats ar$e about "speed" and "hogging" and "blue chips" etc. as I am retired and a couple of extra hours (days sometimes) doesn't concern me at all.

              My tear-ar$ing days are long gone. If I get the urge to get "stuck into it" I just shut the shop and stay out until it wears off. I hasn't happened in a long time!! And it won't happen for a long time yet either.

              Comment


              • #8
                Originally posted by oldtiffie
                I don't give a big rats ar$e about "speed" and "hogging" and "blue chips" etc. as I am retired and a couple of extra hours (days sometimes) doesn't concern me at all.
                I bet you still work the cutter in its "goldilocks" zone...otherwise your probably gonna have premature cutter failure or loss of cutting edge..They need to be worked..

                Rob

                Comment


                • #9
                  Sweet spot

                  Dead right Rob.

                  Every machine, tool and set-up "combo" has its own unique "sweet spot".

                  I feel and listen for it - and when I've got - I go for it.

                  Comment


                  • #10
                    P'raps

                    Originally posted by dp
                    Same thing happens with drills - that's why they make reamers. Perhaps if you had a zero run out mill with an absolutely immobile table and an end mill that was manufactured with zero imperfections regarding symmetry then you may plunge the perfect hole - well, no, that means the work has to be as perfect as your machinery. Not going to happen - use a smaller end mill and machine to spec.
                    Not necessarily so Dennis.

                    The finishing drill will always follow its predecessor as regards where it drills, but its quite easy to get the final drill to drill so close to the size of the drill itself that is it a very neat fit.

                    Leave about 1/64" to drill out on the final cut.

                    Hand-hone small radii along the edges between the cone at the front of the drill (ie the ends of the 118* cone) and the OD of the drill at the flutes.

                    Drill slowly, use plenty of cutting oil, start slowly and when the drill "bites" just push it in and keep going.

                    You just might be surprised at how neat and close to the drill diameter the hole is. The finish won't be too bad either.

                    Spit - yes spit - on your finger and then on the drill works wonders too - t'riffic "cutting oil" - 'specially when starting a "spotting"drill in a centre-punch mark. I always use it - never lets me down. Works well in drilling some hard/tough materials too.

                    I was in my early 'teens when I was taught those ones.

                    Comment


                    • #11
                      Oldtiffie,

                      Is that a morse taper on that milling arbor? I've been looking for one (MT3) for my lathe, but cannot find one. Where did you get it? I'd really rather have a long one to reach the tailstock for extra support, but that'd do.

                      Thanks,

                      Andy

                      Comment


                      • #12
                        If your slotting through a part,drill a hole first with a smaller bit,say 5/16 on a 3/8 slot.Pop in the endmill plunge through and slot.No "keyholes" that way.
                        I just need one more tool,just one!

                        Comment

                        Working...
                        X