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.

CNC Routing Clear Acrylic

Discussion in 'CNC Routing & Laser Cutting' started by Susan Stewart, Jul 14, 2020.

  1. Susan Stewart

    Susan Stewart Member

    50
    7
    8
    Mar 1, 2018
    Indiana
    We have a Laguna Swift 4' x 8' CNC router. We are new to this machine, and we have a few questions that we are hoping someone can help us with. The software we use is VCarve Pro.

    We are routing 1/4" clear acrylic (Plexiglass MC). We routed a program with a depth of .08" @ 18,000 rpm and 54 ipm in 1 pass. The bit we used was Vortex 5609 single edge flute upcut spiral which is supposed to be a good bit for cutting acrylic. It left a lot of melted material around the cut which was difficult to remove. We did cut the acrylic with the protective film on it.

    How can we route this without having the acrylic melt back to itself?
    Are we routing too fast/too slow?
    Should we do a 2nd pass at the same height just to clean the part up?
    Is there a better bit that would give us better results?
    Do we need to remove the protective film before cutting?
     
    Tags:
  2. alevit53

    alevit53 Member

    28
    1
    3
    Apr 20, 2016
    Middletown, NJ
    We use:
    Amana Tool 51404-K Spektra Coated SC Spiral O Single Flute, Plastic Cutting 1/4 D x 3/4 CH x 1/4 SHK x 2 Inch Long Up-Cut CNC Router Bit with Mirror Finish
    It appears you are going too slow and building up too much heat that melts the acrylic.
    We cut straight through 1/4" running at 20000 rpm and at least 100 IPM.

     
  3. Krissy Louderback

    Krissy Louderback Member

    52
    10
    8
    Aug 5, 2019
    Port St. Lucie, FL
    I have a TechnoCNC. I usually use a 1/4" upcut bit, 2 passes, 100ipm, 18000 rpm.
    I think you are running too slow, that's why it is melting together.
     
  4. Andy D

    Andy D Very Active Member

    2,302
    428
    83
    Oct 20, 2014
    Hattiesburg, MS
    It's been many years since I ran a CNC, but I remember this issue.
    Are you blowing away or vacuuming cuttings? When I had to get a perfect edge, I would run the 1st pass
    leaving the cuts 1/32" larger and cut 90% thru the material & run a second pass, removing the 1/32" and cutting 100%
    thru.
     
    • Like Like x 1
  5. LarryB

    LarryB Member

    280
    18
    18
    Dec 3, 2006
    Webster, Texas
    You are running way too slow. Also go with a second pass. We cut 3/16” acrylic with 1/4” bit, 190 speed, 20 plunge, 22000 spindle, 2 pass, conventional cut
     
  6. Cory Marcin

    Cory Marcin Member

    45
    10
    8
    Oct 2, 2018
    Wisconsin
    Agreed. Running too slow. Based on the bit you are using I would be running 1 pass at 20,000 rpm at about 100ipm.
     
  7. Susan Stewart

    Susan Stewart Member

    50
    7
    8
    Mar 1, 2018
    Indiana
    We do have a vacuum attachment on the spindle for the cuttings.

    Sounds like we need to speed it up.

    Thanks!
     
  8. Ian Stewart-Koster

    Ian Stewart-Koster Active Member

    920
    21
    18
    Sep 27, 2003
    Qld, Australia
    Melt and reglue is because of heat.
    Heat is because you are not removing the heat and chips quickly enough - ie X Y speed is too slow. (or conversely cutter RPM is too fast, for the travel speed you are using)
     
  9. Ardor Creative

    Ardor Creative New Member

    20
    5
    3
    Dec 17, 2019
    Worcester, MA
    I go as thin as an 1/8" single flute upcut, either Amana 51445-K or normal plastic bit. Definitely don't unmask the acrylic. I still cut in "climb" for longer bit life, but it's all personal preference.
     
  10. spectrum maine

    spectrum maine Member

    255
    45
    28
    Nov 1, 2012
    biddeford, maine




    are you making chips or dust? always make chips. the heat comes out with the chip.Slow spindle speed down or feed rate up. you can do a first pass very shallow then spray that groove with water from a squirt bottle. (not a lot) then do a deeper 2nd pass. thats how we cut thick aluminum
     
  11. GB2

    GB2 Very Active Member

    1,916
    80
    48
    Nov 15, 2005
    Connecticut, USA
    You are definitely going way too slow, we are routing with a single pass depth of .25" @ 18,000 rpm and 180 ipm with an Onsrud .25 x .625 End Mill 1Flute upcut bit #65-023 on a 13HP Multicam. I'd like to tweak that set up a little too so that we get a more polished finish right off the router but I've been too busy routing jobs to play around trying new bits or settings. Onsrud has some really good chip charts that tell you exactly what settings you should be using for various materials, if you go on-line you can easily find them. They are specifically designed for Onsrud bits but you can use the settings for whatever comparable bit you are using.

    Here's an interesting article about routing plastic:
    https://www.onsrud.com/articles/Fixturing-and-Routing-of-Plastics-with-CNC.asp

    Here's a link to the catalog with the chip charts:
    https://www.piedmontplastics.com/resources/literatures/lmt-onsrud-production-cutting-tools
     
    • Informative Informative x 1
  12. Susan Stewart

    Susan Stewart Member

    50
    7
    8
    Mar 1, 2018
    Indiana

    Thank you for those 2 links. They will come in very handy!!
     
  13. Susan Stewart

    Susan Stewart Member

    50
    7
    8
    Mar 1, 2018
    Indiana
    Thank you all for helping me out. I really like this forum. There is so much knowledge here.

    We did run a small part. On 1/2 of the piece we ran at 50ipm with 12,000 rpm. On the other half we ran at 100ipm with 18,000 rpm. The part with the 100ipm and 18,000 rpm came out nice and clean.
     
    • Like Like x 1
  14. Jester

    Jester Slow is Fast

    106
    18
    18
    Dec 2, 2019
    SoCal
    Last edited: Jul 14, 2020
  15. printhog

    printhog Member

    383
    169
    43
    Dec 15, 2010
    california
    First off know that there are both EXTRUDED and CAST acrylics, and they are totally different beasts in machining settings. Same for aluminum. ALWAYS know your media settings are for the right one. Knowing feeds and speeds for your materials is critical to any quality finish. It is probably the #1 thing to master.

    Each bit has a designed chip size (the bite each pass of the bit takes as it spins- a.k.a. the sawdust size) and a related chip load (how much 'sawdust' chips the bit can clear so the cutting edge has a clear shot at the next site). These relate to the rpm and the forward movement into the stock and the design of the flutes. Its especially true of upcutters. Going over those specs results in problems, but so does going under. You want to drive the bit at 95% of its designed chip load. The data for this is in each bit manufacturer's info sheet. They are all different too. Gerber bits are not the same as LMT-Onsrud for example, even though they may be the same type and design of bit.

    PROTIP - If you are routing clear acrylic, LMT Onsrud makes an ***-kicking diamond finisher that eliminates polishing work or your edges and pocketing.. watch it and weep with joy..
     
    • Like Like x 1
  16. Susan Stewart

    Susan Stewart Member

    50
    7
    8
    Mar 1, 2018
    Indiana
  17. Susan Stewart

    Susan Stewart Member

    50
    7
    8
    Mar 1, 2018
    Indiana

    Thanks! This is great information. Wow! That diamond finisher bit is awesome!
     
  18. fixtureman

    fixtureman Member

    356
    18
    18
    May 16, 2012
    Medina Ohio
    But check out the price.
     
  19. Susan Stewart

    Susan Stewart Member

    50
    7
    8
    Mar 1, 2018
    Indiana
    Holy cow!! That's way too expensive for us.
     
  20. MikePro

    MikePro Major Contributor

    4,974
    235
    63
    Feb 3, 2010
    Racine, WI
    chips need somewhere to go, they'll never go straight-up through the flutes and want to rub/melt against the material as you progress through the shape.

    I'm a huge fan of doing a rough-cut first, anywhere between 0.02"& up to half the diameter of the bit offset from the final part, but leaving .040" remaining in the depth of the material to keep it held in place. then your single-pass final cut will have plenty of room to evacuate chips AND polish the edge as it cuts.
     
    • Agree Agree x 1
Loading...

Share This Page

 


Loading...