Results 1 to 3 of 3

Thread: V90 bit not making clean cuts

  1. #1
    Join Date
    Oct 2015
    Location
    Durham, NC
    Posts
    1

    Default V90 bit not making clean cuts

    Runnning a 1-1/2" v90 bit on white core HDPE at 12K, 1.5 in/sec, leaves burrs on edges and pits on surfaces (see attached).

    Can you suggest better speed and feed settings for this material?
    Attached Images Attached Images

  2. #2
    Join Date
    Jan 2004
    Location
    iBILD Solutions - Southern NJ
    Posts
    7,515

    Default

    There's a few things that come to mind here looking at your photo and settings. The straight run on the right of the pic appears to show the material getting yanked out. This is a clear indication to me that your cut speed is too fast and/or your RPM is too low. Certain plastics can be tricky to dial in, especially grabby/soft ones like HDPE. I would try Zzeroing the bit .02" high (do C2, then MZ,0.02 and ZZ) and cut. Then lower bit to the true Zzero location (easiest is to use VA and add .02 to whatever the DRO says Z is...Like if it says 0.500, put 0.52 in the VA Z field) - then re-cut. With plastics you want to make sure you leave enough meat on the part to shave off cleanly. Sometimes you need a little more like .03-.05 - or the bit will just burnish the surface rather than cut it.

    I would crank the RPM up to 18k and try your same move speed - except I would do the 2-step process outlined above. I am assuming that you have a fresh, sharp v-bit that wasn't used previously on MDF etc. Dull bits in HDPE = failure. Some have suggested Centurion bits in the past, but they may be too small to do what you want. There isn't a lot of variation in grinds between v-bits, but I like the Amana ones for CNC. You can replace the insert as needed. They are single flute & in turn require higher RPM and lower move speed compared to a 2-flute brazed one.

    The other thing that is a possibility is that something is loose on your machine. Since HDPE is grabby, it wants to really pull the machine into the cut. Make sure to shake down your machine and make sure the v-rollers aren't loose and each motor is completely engaged in the rack.

    Try cutting a sample area using the higher RPM and adjust move speeds as necessary. Softer materials do require higher RPM to shear properly, and HDPE has a narrow window. Sharp internal corners will almost always have fuzz because the V-bit just drags at the center of the bit - no cutting or shearing action takes place, so keep this in mind....but tear out like you show shouldn't be happening. Crank that RPM up...

    Post back and let us know how you made out.

    -B
    High Definition 3D Laser Scanning Services - Advanced ShopBot CNC Training and Consultation - IBILD.com

  3. #3
    Join Date
    Nov 2012
    Location
    Lancashire, UK
    Posts
    30

    Default Pass Depth

    Dear David

    Looks like Brady has it covered..

    One thing further you could 'try' is to reduce the pass depth in [Tool] [Edit]. This will help to reduce spelching and prevent the 'grab' as Brady puts it.

    EditTool.jpg

    In good faith
    Martin

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •