Announcement

Collapse
No announcement yet.

Upcut/ Downcut

Collapse
X
 
  • Filter
  • Time
  • Show
Clear All
new posts
  • Upcut/ Downcut


    I tried something today that a machinist friend and I discussed and it worked very well so I though I would pass it along.
    I cut polycarbonate and have always used upcut spiral bits. I use a LOT of screws to hold the material down to the spoilboard to reduce vibration from pulling of the material.
    Today I tried using the upcut for the roughing pass and then switched to a spiral downcut for the 0.03" finish pass and I was able to use 1/3 of the amount of screws for hold-down and the edge finish was the best I've had yet. Since the relief was already there from the roughing pass and I use 2 air blow nozzles, the chips cleared with ease even with the downcut.
    Hope this is useful. Thanks, John
    John Stanley Stinger II 3'x4', FTC, Laser, 1.7 Kw HSD w/ AB 523 SVC drive, V Carve Pro 8, WinCNC
  • #2

    A vacuum hold down system + tooling made for cutting plastic = zero screws + the best edge you've ever seen come off of your tool.

    -B
    IBILD Solutions - High Definition 3D Laser Scanning Services - Advanced CNC Training and Consultation - Vectric Custom Video Training IBILD.com

    Comment

    • #3

      Originally posted by BradyWatson View Post
      A vacuum hold down system + tooling made for cutting plastic = zero screws + the best edge you've ever seen come off of your tool.

      -B
      John, I second what Brady is saying. When I flipped those speaker rings to machine the other side...I used 1/8" aluminum dowels and reset my X0Y0 to be right below one of the inlets for the vacuum hold down. I sent you a response PM, hopefully it went through and you got it.

      Did you glue your spoil board to your plenum by chance?
      Eddie McCullough
      Monroe, NC

      CAMaster Stinger III

      Comment

      • #4

        Eddie,
        Here is a picture of the last batch I did. Parts are 3/8" polycarb; laying side by side. Due to geometry (curves) and ramps (tabs) speed is limited. I roughed at 100 IPM, 10K with an upcut single flute O flute and finished -0.030" with a new Onsrud Super O downcut running 25 IPM @ 10K. I checked run out 1" from collet with an indicator. It was 0.002" max static on the PC 3.25.
        I have run speed/ feed tests from 10 IPM to 100+ but don't have enough straightaway to get to that speed much.
        This is about as good a finish as I have been able to achieve. Any ideas are welcome.
        Thanks,
        John
        Attached Files
        John Stanley Stinger II 3'x4', FTC, Laser, 1.7 Kw HSD w/ AB 523 SVC drive, V Carve Pro 8, WinCNC

        Comment

        • #5

          Originally posted by hefty View Post
          Eddie,
          Here is a picture of the last batch I did. Parts are 3/8" polycarb; laying side by side. Due to geometry (curves) and ramps (tabs) speed is limited. I roughed at 100 IPM, 10K with an upcut single flute O flute and finished -0.030" with a new Onsrud Super O downcut running 25 IPM @ 10K. I checked run out 1" from collet with an indicator. It was 0.002" max static on the PC 3.25.
          I have run speed/ feed tests from 10 IPM to 100+ but don't have enough straightaway to get to that speed much.
          This is about as good a finish as I have been able to achieve. Any ideas are welcome.
          Thanks,
          John
          John,
          I think those look pretty good for only using a single flute. Have you tried a two flutes or more for your finish pass? Also, I noticed that I think the .03" allowance was a little too much, but I didn't do very much testing with the finish pass. When I left .03", it almost seemed like the flutes (I used a 3 flute low helix finisher) had too much material to take off.

          I'll try to take up close pictures like you did.
          Eddie McCullough
          Monroe, NC

          CAMaster Stinger III

          Comment

          • #6

            No, I just use the one that Martin @ Onsrud recommended. I used to do a 0.015 finish pass and he indicated 0.030 was prefereable to load the bit properly and reduce susceptabilty to heat. I can't remember if it helped but it didn't hurt so I stayed with it.
            I will look to see if they have a 2 flute cutter for polycarb.
            Xray, Gary- any thoughts?
            John Stanley Stinger II 3'x4', FTC, Laser, 1.7 Kw HSD w/ AB 523 SVC drive, V Carve Pro 8, WinCNC

            Comment

            • #7

              Originally posted by hefty View Post
              No, I just use the one that Martin @ Onsrud recommended. I used to do a 0.015 finish pass and he indicated 0.030 was prefereable to load the bit properly and reduce susceptabilty to heat. I can't remember if it helped but it didn't hurt so I stayed with it.
              I will look to see if they have a 2 flute cutter for polycarb.
              Xray, Gary- any thoughts?
              I received the opposite information from Onsrud. Bob at Onsrud recommended the Onsrud 60-249 (thats the 3/8" 3 Flute Low Helix Finisher) and taking off .004" on the finish pass, 18000 @ 200ipm. Experience told me that .004" was not enough for a finish pass but I did use the rpm and ipm. If I was in your position, I would get the 60-249. But you might have to play around with speeds and feeds due to polycarb...in my experience it melts at about the same rate as extruded acrylic.

              Attached is a picture of my finish pass. I can't take a closer picture because the camera will not focus that close. I think the biggest difference here is my triple flute low helix.
              Attached Files
              Eddie McCullough
              Monroe, NC

              CAMaster Stinger III

              Comment

              Working...
              X