Announcement

Collapse
No announcement yet.

keyseat milling & burrs

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

  • keyseat milling & burrs

    'morning gang. question to follow..

    got a little "work": 1" x 8" long 1040 shafts with 8mm key cut for 3.5".
    doing 40 pieces.

    Endmill running just shy of 2k rpm (1800 according to the plate), feed
    approx 4.5 ipm.. DOC ~ 0.055" per pass. Cutting the whole keyseat
    in 3 passes down to 0.160" deep. Flood coolant and HSS endmill.

    results look good.. taking me about 10-12 minutes per shaft.
    that sound about right? those feeds/speeds seem reasonable?

    real question: after about 6 shafts or so ... or about 20" keyseats cut
    i'm raising one hell of a burr on one side.. probably 1/8" tall. assumed
    my cutter was dull and time for a new one (which means 6 endmills to
    do 40 shafts!!) .. but on close inspection the edges look perfect.

    The flutes still "catch" my fingernail.

    So I guess thats probably no way to check endmill sharpness.. but I've
    never done a 'production run' before

    Anything I can do to minimize that burr? Its a real bugger to get off.
    Hitting them on the belt grinder leaves less than professional looking
    results... I peel them off with a handfile.. they look nice.. but takes
    time.

    Thanks
    Tony

  • #2
    ps its a 2 flute center cutting endmill.
    I'm plunging straight down 55 thou then power feeding.

    I know thats not the greatest way to do, but i started off
    roughin with a 1/4" mill and then sizing with the 8mm but
    it just took too long and results with just going in the 8 are
    pretty darn good.

    This isn't my day job, but it be nice to at least make enough
    $ to buy the endmills I need to do the job.

    Comment


    • #3
      I think the cutter rpm is to high my rough calc. give me 980 rpm for that size cutter


      but I may be wrong as I have been in the past


      Stuart

      Comment


      • #4
        I think you are running that endmill 2x as fast as it needs to be, and I'd do it in one pass rather than three (why just dull the bottom 50 thou?) with flood or at least air to get rid of the chips.....if the mill can't do it in one pass, slow down the rpm and feed until it can....but really you've got the wrong tool......use a keyseat cutter...or for real luxury get a horizontal mill

        seriously, end mills do a rotten job of keys. A key seat cutter will do a much better job, spot on dimension and minimal burr.

        if you get one, do your speed calculation first and it will last the job....else you'll burn it up!
        Last edited by Mcgyver; 06-02-2012, 09:43 AM.
        .

        Comment


        • #5
          Hello,

          I've never been able to get a good finish or accuracy plunging in multiple passes on a slot. A toolmaker friend of mine says the cutter wants to push and pull into the sides of the slot as it takes a bite. Kind of like oscillating between conventional and climb milling all in the same cut. I know you have to do it sometimes though especially on a vertical mill. Speaking of.... could you hold the part sideways and cut it with an 8mm saw on an arbor (maybe even in one pass with slow powerfeed)? Might be overkill, just an idea.

          Are you getting accurate slots with nice finish other than the burr? If so you could take an angle cutter or large radius ball mill and make a pass to clean up the edge burr. (Kind of like power filing!)

          KEJR

          Comment


          • #6
            Hi,

            I agree, turn the speed down to 1000rpms or just a bit under. Cut the keyway to full depth in one pass. I find a 4-flute will tend to give me the best finish and accuracy for size, BUT you need careful to keep the slot clear of chips. Since there isn't as good of chip clearance.

            Are you using a coated M42 endmill? If not, you may wish to reduce your feed rate down to 2 1/2" to 3 1/2" ipm to increase tool life.

            There is more to flood cooling than just pouring coolant on the cut. There does need to be enough pressure to remove the bulk of the chips as you cut. If you aren't achieving that, you need to figure something out. Whether it's more pressure or using a chip brush to wipe the area.

            dalee
            If you think you understand what is going on, you haven't been paying attention.

            Comment


            • #7
              Thanks guys. Correction, though, I read the nameplate wrong I was/am
              running at 920rpm.

              As a hobbyist I tend to go by ear/experience. Turns out I was being
              too conservative with chip load.

              Opened my coolant valve all the way up (lots of flow, not alot of pressure..
              might have to rig up a smaller nozzle.. this one is probably 3/16")

              anyway, at full DOC, 920rpm, coolant full throttle I've built my confidence
              up slowly from 2ipm back to 4ipm -- don't think I want to push my luck
              any more, but I'm chewing thru these shafts at under 5 mins each.

              PS a flap wheel for the bench grinder, 120gr does a stellar job of
              knocking the burr off without screwing with the finish. I run a round
              file around the inside perimeter and I'm golden.

              Thanks again!

              Tony

              Comment


              • #8
                Judging from some of the posts it time for a rant:

                Back when serving my time (Spring, 1962) Don Herman taught me to cut a key seat with an undersized endmill going down the center to length and depth. Then side shift and climb cut the sides to width if the machine will do it without the table lungeing into the backlash. The reason for this was cutter deflection which can be considerable. Examine the hesitations and ends of the cut. You will see little divots where the cutter dwelled and the cutter deflection relaxed into the sidewall.

                A keyseat cut with an on-size endmill to full width and depth in a single pass may be acceptable if done without hesitation at a constant feed. The small amount of assymatry may go unnoticed at assembly.

                When you cut a keyway or any other feature where the elasticity of an endmill or other cutter plays a part in the operation you still have to consider cutter deflection. The effect of deflection is there, can be seen and measured and is therefore a fact. Thus, deflection has to be acknowledged, understood, and allowed for.

                1 - what we'll call for now the "three pass method" will cut a centered keyseat to size and on center

                2 - the "single pass method" will cut a keyseat displaced laterally by the amount of the cutter deflection leaving divots in the wall representing hesitations, varying feed rates, and dwells.

                I pass this on for noobs and hobbyists who may not have been mentored in this little detail of keyseat cutting. Those wedded to the "single pass method" may take exception. I only ask that they cut a few sample keyseats using both methods and measure the results before refuting my words.

                Time is not everything if the result is uninteded assymetry, irregularities in the walls of stressed features, and uncontrolled processes whose results are visible to the naked eye. The customer may notice the funny keyseat; he may say nothing if the key fits but he may send future work to another shop leaving you without feedback.

                Addressing the burr question. Your cutting edges may be pooping out or you may be re-cutting chips friction-welding them to the wall. In the first case, replace the cutter. In the second purge the cutof chips with forcible coolant flow, a small diameter blast of compressed air, or vacuum them up as they are generated.
                Last edited by Forrest Addy; 06-03-2012, 03:23 PM.

                Comment


                • #9
                  Originally posted by Forrest Addy
                  Judging from some of the posts it time for a rant:

                  Back when serving my time (Spring, 1962) Don Herman taught me to cut a key seat with an undersized endmill going down the center to length and depth. Then side shift and climb cut the sides to width if the machine will do it without the table lungeing into the backlash. The reason for this was cutter deflection which can be considerable. Examine the hesitations and ends of the cut. You will see little divots where the cutter dwelled and the cutter deflection relaxed into the sidewall.

                  A keyseat cut with an on-size endmill to full width and depth in a single pass may be acceptable if done without hesitation at a constant feed. The small amount of assymatry may go unnoticed at assembly.

                  When you cut a keyway or any other feature where the elasticity of an endmill or other cutter plays a part in the operation you still have to consider cutter deflection. The effect of deflection is there, can be seen and measured and is therefore a fact. Thus, deflection has to be acknowledged, understood, and allowed for.

                  1 - what we'll call for now the "three pass method" will cut a centered keyseat to size and on center

                  2 - the "single pass method" will cut a keyseat displaced laterally by the amount of the cutter deflection leaving divots in the wall representing hesitations, varying feed rates, and dwells.

                  I pass this on for noobs and hobbyists who may not have been mentored in this little detail of keyseat cutting. Those wedded to the "single pass method" may take exception. I only ask that they cut a few sample keyseats using both methods and measure the results before refuting my words.

                  Time is not everything if the result is uninteded assymetry, irregularities in the walls of stressed features, and uncontrolled processes whose results are visible to the naked eye. The customer may notice the funny keyseat; he may say nothing if the key fits but he may send future work to another shop leaving you without feedback.

                  Addressing the burr question. Your cutting edges may be pooping out or you may be re-cutting chips friction-welding them to the wall. In the first case, replace the cutter. In the second purge the cutof chips with forcible coolant flow, a small diameter blast of compressed air, or vacuum them up as they are generated.
                  Second the idea of using an undersize endmill and cleaning up the sides on following passes.
                  Deflection can be considerable enough to leave you with kidney bean shaped slots.
                  Deburring will be less work as the burr on one side will be minimized by the following pass.

                  Comment


                  • #10
                    Hi,

                    I often use undersized endmills to cut keyslots in three passes. But it all depends on the fit required.

                    Not much sense in wasting time and money with a close tolerance fit if the size only needs to be -.000/+.005. Just make sure you understand what's required and when it's required.

                    dalee
                    If you think you understand what is going on, you haven't been paying attention.

                    Comment


                    • #11
                      My comments are after a lot of recent slotting, not years of experience. I agree that deflection means you must cut down the centre and finish both sides later if you want to avoid dwell at each end.

                      And on the second and third pass you'll be cutting chips twice. This is because you're cutting in a slot that is already there. The first pass, you're not cutting chips twice, because the chips in front of the cutter are sitting on the surface, and you're not going to cut anything above the surface. So, as Mcgyver said, you'll get more out of your cutter by doing the slot in one pass. Of course deflection will be worse, hence even more need to do a central pass and two clean up passes.

                      Slots with a horizontal mill are much nicer, if the ramp at the inner end is acceptable, although you'd need something pretty hefty to do 8mm in one pass. Two 3mm passes, one on either side, with a central pass later is how I'd do it.
                      Last edited by rohart; 06-03-2012, 09:59 PM.
                      Richard - SW London, UK, EU.

                      Comment


                      • #12
                        A little blast of air will clear those chips right out, no worries.

                        Comment


                        • #13
                          Thanks all for the tips.
                          Managed to work through rest of job pretty quick.

                          Don't quite get it: first 10 pcs took 1 1/2 endmills. After reading
                          some responses here and pushing through with false confidence I managed
                          to do the rest (another 30+) with just one endmill. And its still in
                          one piece and has its corners.

                          PS quick tip if anyone is looking to easily downside their coolant nozzle:
                          heat shrink! worked perfect, can shrink it down to the size you need and
                          not a sweat if it gets buggered.

                          Thanks again
                          Tony

                          Comment


                          • #14
                            That's often the way it goes with me too. I think it's because if you're not an expert then you mess up the endmill not on the standard long haul but on that few thou at the end, that few thou milling over an edge without tightening down the gib, where it touches into climbing briefly.

                            I had a habit of drilling a starter hole at both ends of my slot - basically because I hadn't decided whether to saw each side and clean up with the mill, or do the whole job in the mill. Well, when the endmill gets to the terminal hole, if I don't tighten my gib lock screw briefly all hell breaks loose, and it sounds like pulling teeth.

                            Those little mistakes are what knacker cutters in a mill, IMO.

                            That's why I prefer turning, for the moment, anyway.
                            Richard - SW London, UK, EU.

                            Comment


                            • #15
                              Originally posted by rohart
                              ...<snip>

                              And on the second and third pass you'll be cutting chips twice. This is because you're cutting in a slot that is already there. The first pass, you're not cutting chips twice, because the chips in front of the cutter are sitting on the surface, and you're not going to cut anything above the surface. So, as Mcgyver said, you'll get more out of your cutter by doing the slot in one pass. <snip>

                              .....
                              I would disagree that you do not cut chips twice on the first cut. There is nothing to stop chips in the slot behind the cutter from being swept into the cutting area. And chips on the cutter itself.

                              IMHO, the only way to prevent this is to use either air or coolant flow to remove the chips from the area.
                              Paul A.

                              Make it fit.
                              You can't win and there is a penalty for trying!

                              Comment

                              Working...
                              X