Announcement

Collapse
No announcement yet.

Feed Rate for 1/16th" Endmill

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

  • Feed Rate for 1/16th" Endmill

    I have to cut a some 2x2mm fins in some 6061 (tiny heatsinks) and my feed/speed chart does not go down that far. I have a couple of 2 flute stub length HSS endmills and a spindle that goes up to 8000 RPM. Anyone know a safe but efficient feed rate with full flood coolant?

  • #2
    I use around .0005" chip load for .062" end mills at about .032 DOC at 7500 rpm. A two flute EM at 8000 rpm would feed at 8. IPM. Keep lots of coolant flowing to clear the chips.
    Mark Hockett

    Comment


    • #3
      Climbing?

      Mark,

      "climb" or "conventional" milling? (To assist with swarf clearance).

      Comment


      • #4
        Originally posted by oldtiffie
        Mark,

        "climb" or "conventional" milling? (To assist with swarf clearance).

        Always climb on CNC mills.
        Mark Hockett

        Comment


        • #5
          Originally posted by MickeyD
          I have to cut a some 2x2mm fins in some 6061 (tiny heatsinks) and my feed/speed chart does not go down that far.
          Mike, that's because with such a tiny endmill in aluminum, your SFPM is essentially infinite.

          I.e., for a 0.0625" endmill in Aluminum, which is recommended as 650 - 1200 SFPM, you need to run at 30,000 - 60,000 RPM.
          So the tooth load calculation is going to be based on essentially "infinite" spindle speed.

          Bottom line: no matter how fast you run the spindle, your VMC isn't going to hit the minimum 0.001" per tooth load that's usually recommended...
          Last edited by lazlo; 12-22-2008, 05:19 PM.
          "Twenty years from now you will be more disappointed by the things that you didn't do than by the ones you did."

          Comment


          • #6
            Lazlo,

            First off, love your signature.

            I've been working with 1/8 solid carbide endmills in A2 steel suing the highest speed on my Bridgeport which is 2720 RPM's. Too slow by the book but worked great although could only do .030 at a time due to the little bugger wanting to deflect. Feed rate adjusted by eyeball.

            I ran a .25 solid carbide endmill at .100 depth of cut and about 1800 rpm's and it worked great although the feed rate was probably only 2 IPM.

            The 1/16 is probably a whole 'nother beast and it is sure to want lightning fast speeds.

            --Cameron

            Comment


            • #7
              I normally try to run everything except facemills and flycutters at 7500 on aluminum when I am running coated tools. It is a lot of fun watching a half inch em running at 120IPM plus.

              Comment


              • #8
                Originally posted by Mark Hockett
                Always climb on CNC mills.
                Totally unrelated to the thread, but I have found that with long series endmills I get a better finish and less chatter if I conventional mill the finish pass on the CNC. By long endmill I'm saying like a 2" or 3" cutting length 1/2" endmill. Maybe this is common knowledge, not sure, otherwise always climb like you said.

                Comment


                • #9
                  I do a lot of milling with 1/8 and 1/16 solid carbide endmills. I finally stopped breaking them when it dawned on me to feed them at the same proportionate rate for their size as a much larger tool. If you were cutting the same material with a 1/2" endmill and it took 3 seconds to cut though 1 diameter worth of material the use the same rule for the small sizes too. In other words, feed it at the same number of seconds per diameter.
                  Free software for calculating bolt circles and similar: Click Here

                  Comment


                  • #10
                    If I was making heatsinks I'd see if I could do it with a table saw and carbide blade. I haven't done it yet but in a recent thread I started guys say it works great. I bought a blade to try it on but have not mounted and tested it out yet. You probably know if you have the heat sink black anodized it will dissipate the heat better.
                    - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - - -
                    Thank you to our families of soldiers, many of whom have given so much more then the rest of us for the Freedom we enjoy.

                    It is true, there is nothing free about freedom, don't be so quick to give it away.

                    Comment


                    • #11
                      Question??? Why do you climb mill with CNC?
                      I have tools I don't even know I own...

                      Comment


                      • #12
                        Russ,
                        There are a bunch of reasons for climb milling, one is to prevent re-cutting chips which gives you a much better finish and makes the cutter last much longer. It reduces work hardening. It pushes the cut toward the work holding device instead of trying to push it away, and less power is needed to make the cut.
                        The reason climb milling works on CNC machines is no backlash. If you take heavy climb cuts on a manual machine the cutter can grab and do a lot of damage.
                        It is also the reason I rarely use carbide on my BP. Carbide end mill cutting edges chip very easy when re-cutting chips which causes them to fail much quicker. On my CNC equipment carbide lasts much longer, to the point I will wear them out before I ever get a chip on the cutting edge.

                        An experiment you can try on a Vertical mill is make a conventional cut and look at the finish, then feed a couple of thou on the radial depth of cut and and make a climb cut back over the conventional cut about half way across, then compare the finish.
                        Last edited by Mark Hockett; 12-22-2008, 09:55 PM.
                        Mark Hockett

                        Comment


                        • #13
                          Climb milling

                          Mark is "spot on".

                          Russ, for an explanation, see the text and graphics at:
                          "Conventional milling versus climb milling" about the bottom of the page at:
                          http://en.wikipedia.org/wiki/Milling_cutter

                          Comment


                          • #14
                            Ooops..I already knew the differences between the two...I just was wondering why only climb milling with a cnc.
                            I "was" going to say..."Isn't milling...milling?" But now I know!
                            Thanks for the explanation!
                            Russ
                            I have tools I don't even know I own...

                            Comment


                            • #15
                              I have a handful of 4 flute carbide end mills, but they gum up with 6061 (been there and done that) and there were only 3 2 flute end mills in town. I would love to cut the slots on a saw, but the tolerances are just too tight. The fall back was that I could do them on the shaper, but the mill will be easier and more accurate.

                              On the subject of climb vs. conventional milling on a cnc, climb milling really does give a nicer finish and helps to avoid material welding to the flutes and causing tool breakage.

                              Comment

                              Working...
                              X