Welcome To Signs101.com: Largest Forum for Signmaking Professionals

Signs101.com: Largest Forum for Signmaking Professionals is the LARGEST online community & discussion forum for professional sign-makers and graphic designers.

 


  1. This site uses cookies. By continuing to use this site, you are agreeing to our use of cookies. Learn More.

broken 1/16th endmil in 1/8' acrylic

Discussion in 'Dimensional Signs' started by iSign, Feb 16, 2011.

  1. iSign

    iSign Major Contributor

    13,027
    31
    48
    Nov 29, 2003
    Kahului, Maui
    I used 2 passes, 150 IPM feed, 60 IPM plunge, and 18000 rpm spindle..

    I also used a 3D "line in" in enroute (meaning the bit plunges & begins to advance simultaneously, instead of drilling a hole and trying to advance against the full depth from a dead stop...

    as you can see in the pics, I made it through several pieces, but 80% of the way to completion I broke another tool...

    any suggestions?
     

    Attached Files:

    Tags:
  2. Jet Fast Printing

    Jet Fast Printing Member

    384
    1
    0
    Sep 22, 2009
    Have you tried calling Onsrud directly? I had issues just like yours before and they had me slow it down and wa-laa stopped breaking bits.

    800-234-1560 <----- Onsrud
     
  3. signmeup

    signmeup Major Contributor

    7,468
    13
    38
    May 5, 2005
    Canada
    I have no router so take this for what it's worth.. could spinning something that small, that fast, snap it if it was even the tiniest bit out of balance? If it went harmonic it would dissappear, I would think. Again, I have no idea how much would be sticking out of the collet.
     
  4. Typestries

    Typestries Very Active Member

    1,581
    4
    38
    Jan 8, 2007
    NJ | VT
    For a 1/16th bit I think your feed rate is waaaay too high even for 2 pass cutting. Like 100 too high, as is the plunge.

    It could also be a vibration issue. Any chance the piece is vibrating as it's cutting, small bits are very susceptible to vibration breaks.

    Reducing the speed to something like 30 ipm might also reduce potential vibration.

    Do they break in the same spot on the shape?
     
  5. J Hill Designs

    J Hill Designs Major Contributor

    15,549
    16
    0
    Sep 24, 2004
    also, I would never use a 1/16th bit in 1/8' (1.5") acrylic

    haha j/k :thumb:
     
  6. GB2

    GB2 Very Active Member

    1,918
    81
    48
    Nov 15, 2005
    Connecticut, USA
    I agree, way too high feed and plunge rate, everything else seems OK though. Those bits get expensive fast don't they?!
     
  7. m giese

    m giese Member

    41
    0
    0
    Nov 20, 2009
    Cast or extruded ACR?

    General rule of thumb with acrylic cutting is the cut depth/pass should be half the d of the tool.

    I have found that a plunge rate of 15-20, and a feed ipm of 120-140. At slower speeds I start to have reweld issues.

    The other factor that can come in to play is acceleration rates. Too high, too much stress on the tool

    The key to the small d tools seems to be in minimizing the stress on the carbide by cutting down on the pass depth.

    Of course, a larger d tool couldn't hurt, but I assume you choose the 1/16 tool for a reason.
     
  8. m giese

    m giese Member

    41
    0
    0
    Nov 20, 2009
    Just looked at your images, couple of thoughts...

    if you are cutting w vac hold down, you may be getting to much vibration and movement, as another poster suggested. based on the close proximity of the newly created holes, ie part to part distance. Hold down looks better near the beginning, and becomes an issue farther down the nest.

    For the delicate work, switch to paper masked material instead of the film, doesn't wrap up around the tool, and stays in place until you choose to remove it. Use the 1/16 bit for the inner, smaller geometry, and switch to a .125 end mill for the outer geometry, obviously changing your tool paths, and last but not least when using the 1/16 to cut the inner geometry, keep the kerf cleaned out with some air, particularly on the subsequent depth passes.
     
  9. signs2trade

    signs2trade Active Member

    Good suggestions here.

    You may also try maxing out the RPM of your spindle. The faster you spin the smaller bits the stronger they effectively become.
     
  10. iSign

    iSign Major Contributor

    13,027
    31
    48
    Nov 29, 2003
    Kahului, Maui
    Thanks for the tips guys...

    I assumed the 1/8" tool would spoil the detail, but it actually didn't compromise the design nearly as much as I thought... But more passes, with slower feed and faster rpm is my lesson here...

    The words "acceleration rate" was used, below mention of feed rate by the same person, what does that mean, if not the same as " feed"
     
  11. m giese

    m giese Member

    41
    0
    0
    Nov 20, 2009
    Acceleration rate is the rate that the tool accelerates in movement from the initial plunge, if you are not using ramping. IE, tool plunges at entry point, and then accelerates to feed speed, decelerates at direction changes in geometry. May or may not be a setting you have control over, but high acceleration rates contribute to tool breakage, especially with smaller diameter carbide bits.

    If you need any spare packaging for those 63-700's I have a few you could add to your pile...

    - Mark
     
  12. iSign

    iSign Major Contributor

    13,027
    31
    48
    Nov 29, 2003
    Kahului, Maui
    Thanks Mark!

    I use Enroute 4, and I don't remember noticing acceleration adjustments, but that makes sense that it doesn't hit top speed from the get go, and also makes sense that having control is a good thing... so I'll expect to find it now that i plan to look...

    regarding the packaging... glad to hear I'm not alone building up a little stack... just think, soon we'll have enough to recycle into justifying one more bottled soda consumption!
     
  13. Design4cnc

    Design4cnc New Member

    6
    0
    0
    Jun 7, 2011
    I know this is very late to the post date but your accel speeds would be in actual router settings or in router post. What kind of CNC do you have?
     
  14. iSign

    iSign Major Contributor

    13,027
    31
    48
    Nov 29, 2003
    Kahului, Maui
    Hi D4CNC,
    I have the Multicam 3000 series
     
  15. k.a.s.

    k.a.s. Very Active Member

    1,411
    4
    38
    Aug 8, 2003
    NE ohio
    I have had zero success with 1/16 inch bits, if it cant be done with an 1/8 it needs to be done on a laser. JMO


    Kevin
     
  16. astro8

    astro8 Active Member

    778
    17
    18
    May 23, 2009
    Sydney, Australia
    Your speeds were far too high, about x5 too high! Those little bits even though spinning at 18000 rpm don't have much surface speed at the cutter. If you have a mister it helps to blow just the air over the tool on acrylic but with water will give you a better edge.

    We do a fair bit of cutting with 1/16" bits on our router, aluminium, brass, acrylic, mdf, acp. Even taking all precautions, ramp ins, acceleration adjustments, they don't last all that long...buy them in boxes of 50 at a time.
     
  17. daveb

    daveb General Know-it-all

    249
    0
    16
    Feb 11, 2010
    Quincy, IL
    I used to use 3/32'' bits for cutting small stuff, tried 1/16'' and ran through a ton of them and then Hartlouer suggested using the 3/32'', worked like a charm. I was routing 080 alum. faces which is probably a lot different than what you're doing. You do however sacrifice a "little" detail. Always talk to your supplier, they know their product and should be able to point you in the right direction. Hartlauer was always very helpful, of course it has been several years since I was in the router room full time but I don't think much has changed.:rolleyes:
     
  18. 88flstf

    88flstf New Member

    5
    0
    0
    May 25, 2011
    try this

    I had a lot of 1/16" bits break... just look at them at they break. Then Hartlauer suggested that the problem was the 1/4" shank and so I switched to the 1/8" shank with a 1/8" collet and presto... no more broken bits. They just get dull now. But you still have to run and plunge quite slowly even with running at 24,000.
     
  19. iSign

    iSign Major Contributor

    13,027
    31
    48
    Nov 29, 2003
    Kahului, Maui
    boggles my brain how much I have to learn...

    but it's a pretty mind boggling reality how much information is available to learn here... so, one day at a time...

    by the way, what those cuts were for is a little side project I started fitting in after other router jobs were getting done over a few weeks time... I decided to invest 3 or 4 square feet of each of several materials, including even some Koa exotic hardwood material I ran through a planer... and I came up with a few dozen material sample fandecks to use as a sales tool with the highest end clients like resort properties, as well as for possibly branching out into offering wholesale services to my competitors.

    Anyway, here are the finished products:

    [​IMG]

    [​IMG]
     
  20. Mainframe

    Mainframe Very Active Member

    Cool sample, I like it, nice work!
     
Loading...
Similar Threads - broken 16th endmil
  1. Nehal

    Need Help Suggestions Discussion Question Opinion HP Latex L26500 Broken Bag Error26.4:10 or 13.2:10 or 01.2:10

    Replies:
    9
    Views:
    612
  2. Texas_Signmaker
    Replies:
    62
    Views:
    1,905
  3. ml4cs
    Replies:
    11
    Views:
    512
  4. KH t's n Signs
    Replies:
    1
    Views:
    678

Share This Page

 


Loading...