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.

Edge finish on ACM

Discussion in 'CNC Routing & Laser Cutting' started by CanuckSigns, Oct 30, 2020.

  1. CanuckSigns

    CanuckSigns Very Active Member

    3,506
    430
    83
    Nov 11, 2008
    Ontario
    I am running a summa F1612 with the standard router attachment, still learning the ropes when it comes to routering.

    I am running some 6mm thick ACM and the edges are not coming off the machine looking very good, it's leaving behind little strands of plastic that need to be sanded off.

    My settings are:
    4 mm O flute upcut bit
    spindle speed - 25,000 RPM
    Feed speed - 1.5 inches/min
    2 passes with a clean up pass at the end
    Climb cutting

    When I cut 1/8" ACM with similar settings I get perfect edges with no clean up needed.

    Can anyone more familiar with CNC routing ACM take a look at the attached pic and see if you can think what is causing this?

    Cheers!
     

    Attached Files:

    Tags:
  2. JBurton

    JBurton Signtologist

    2,001
    441
    83
    Sep 28, 2017
    Arkansas
    Are you sure about that 1.5 inches/minute?
     
  3. CanuckSigns

    CanuckSigns Very Active Member

    3,506
    430
    83
    Nov 11, 2008
    Ontario
    Whoops 1.5 inches/sec
     
  4. Wesley Powell

    Wesley Powell Account Rep

    35
    5
    8
    May 29, 2018
    Lima, OH, USA
    I've had good success cutting ACM at 18,000 rpm and about 180in/min. For 3mm I'll just do a single pass, for 6mm I'll do 2 and call it good.
     
  5. MikePro

    MikePro Major Contributor

    5,042
    259
    83
    Feb 3, 2010
    Racine, WI
    bigger bit, would be a good start, RPM's seem a bit high. I only use 1/8" bits when cutting detailed lettering, but if I were to be using it for 1/4" ACM I would be running at 19000 climb and only .063-080" per pass. big fan of using 1/4" bit for all of my square-panel cuts and especially on thicker materials.

    pardon my use of non-metrics, but if you're looking for pristine edges on ACM I'd tread it like it is: two layers of .040 alum with a buncha soft plastic in-between. 1/4" upcut bit (bonus points for using one intended for aluminum), rough cutting 3/16" deep @ -035"-..125" offset from true shape (to give room for alum/plastic chips to evacuate) and then true shape cut being 3 passes at .090". It will clean cut the face, then clean cut the core, then clean cut the opposing face, with plenty of room for evacuation.
     
  6. JBurton

    JBurton Signtologist

    2,001
    441
    83
    Sep 28, 2017
    Arkansas
    This seems crazy, I don't think I've ever cut acm in more than one pass, but I'm using belin 33317a upcut single flute bits, used primarily for aluminum. I've done what MikePro is suggesting, but only on stuff like 3/4 acrylic.
    Try running closer to 18-19k rpm, 60 inches/minute. Also, depending on your bit shape, clockwise/counterclockwise makes a big difference. Of course you'd notice that your drop has a pristine edge and your part is fuzzy...
     
    • Informative Informative x 1
  7. MikePro

    MikePro Major Contributor

    5,042
    259
    83
    Feb 3, 2010
    Racine, WI
    ya i run Belin's too. 1----'s on plastic, and 3----'s on aluminum/acm.
    Agreed that 4 passes to cut a square out of ACM is bonkers, but I still think this issue is chip evacuation & exaggerated by higher rpm's. I'm also using rough&multiple passes on the regular since my cuts are mostly 1/2" acrylic, and .125"-.5" aluminum, and my randomly blurted-out info may be overkill :)
     
    • Agree Agree x 1
  8. JBurton

    JBurton Signtologist

    2,001
    441
    83
    Sep 28, 2017
    Arkansas
    Ah, good. It's been a long week, this had me questioning my sanity! Say, what are you using for lubricant/coolant on your aluminum? I've been running kool mist for a couple of years now and it's great, except when I have to cut something with multiple passes like 1/4" aluminum, I end up with so much fluid on the part that it actually seems to impede cooling. We used to run trico micro mist lubricants, which worked better, just pricier, and it constantly gummed up the mister unit. Then we discovered alcohol and never looked back. But cost of alcohol being what it is, we found kool mist and it works comparably, just doesn't evaporate anywhere near as quickly.
     
  9. alevit53

    alevit53 Member

    30
    2
    8
    Apr 20, 2016
    Middletown, NJ
    We cut ACM with a coated aluminum 1/8" upcut bit. 18000rpm and 150 ipm. One pass with slope insert.
    Too slow and the plastic melts.
    If you are talking about Alumalite, that's a different story. We use
    Amana Tool 46302 CNC Solid Carbide ZrN Coated Honeycomb Cutting 1/4 D x 3/4 CH x 1/4 SHK x 2-1/2 Inch Long, 6-Flute Router Bit
     
  10. Michael-Nola

    Michael-Nola I print things. It is very exciting.

    51
    12
    8
    Jul 21, 2016
    20874
    ACM is literally swiss cheese. Regardless of bit, you should be running 1 pass with only evacuation being your reducing rate. 3/16" bits should be running 50k rpms at 400ipm. 25k baby spindles should run 200ipm. It's all math and sound. Routing is not an unskilled labor. Get a proper speeds and feeds textbook with algebra in it. Drop perfected methods into your cutting keys and push through hundreds of sheets per day.
     
  11. MikePro

    MikePro Major Contributor

    5,042
    259
    83
    Feb 3, 2010
    Racine, WI
    been using the TriCool vegetable based (green label) lubricant for over a decade now... love it! Agreed that its a bit pricey at $125/gallon, but that gallon goes a long way through the mister. My CNC runs about 30hrs a week on aluminum parts, and i'll go through maybe a gallon every three months. I've tried the synthetic stuff (redlabel), which is cheaper by the gallon BUT its more liquidy and even at the lowest setting it still feels like it just pours out of the mister and leaves the routed parts absolutely bathed in oil and i'll go through that gallon about 3x as fast.
     
  12. JBurton

    JBurton Signtologist

    2,001
    441
    83
    Sep 28, 2017
    Arkansas
    It is great stuff, but keeping it flowing just right was my biggest issue. What's your misting unit? I was using a Trico MD1200 for years, but kept cracking the reservoirs after the first one went out. Like 1 reservoir lasted 10-20 years, the next 3 each lasted 6 months.
     
  13. MikePro

    MikePro Major Contributor

    5,042
    259
    83
    Feb 3, 2010
    Racine, WI
    still same Trico MD1200 unit here.... installed when we bought the CNC ~15yrs ago. I've had to replace the mister tips a few times, after they occasionally make contact with the spindle and grind-down on the tip, and recently did a major overhaul to re-fit the entire setup with new oil lines (lawnmower fuel lines are the same guage/material for the mister unit), but otherwise its been rock-solid. Would highly recommend anyone machining aluminum parts on their CNC to do so with a mister. Not necessary for ACM, however, regarding the OP. Don't think i've ever routed ACM with the oil mister, nor felt the need to try as its pretty much just plastic with a foil coating.
     
    • Like Like x 1
  14. Grizzly

    Grizzly Member

    185
    20
    18
    Sep 1, 2010
    Utah
    It looks like this is laminated. If so, the adhesive can cause the chips to stick and leave the appearance your showing. Is it possible to route from the back side? We have a flip/cut feature on our Zund that helps with laminated products.
     
Loading...

Share This Page

 


Loading...