Having serious aluminum trouble!

New Home Forum Mostly Printed CNC – MPCNC Troubleshooting – MPCNC Having serious aluminum trouble!

Tagged: 

This topic contains 12 replies, has 4 voices, and was last updated by  Ty 2 months, 3 weeks ago.

Viewing 13 posts - 1 through 13 (of 13 total)
  • Author
    Posts
  • #94396

    Ty
    Participant

     

    Ok, so I’ve been really frustrated, I originally had a little dremel 100 on my mpcnc, it was weak but i seemed to get the settings dialed in to where i could cut aluminum an wood quite well. However since upgraded to the dw660 ive had nothing but headaches when i comes to aluminum. I have quite a small machine, 24″ x 26″ and 3″ of z travel, but since upgrading my router i’ve not been able to cut aluminum constantly at all! I’ve tried every setting in the book, both linear and trochoidal milling, although linear has worked in a few cases, it does not work inconstantly. The main thing I am observing that causes the cut to fail is overheating of the aluminum and the cutter, even if i add oil constantly it still wont complete a proper cut. the only way i can seem to get a cut is if i don’t use trochoidal, and i go extremely slow, like 4mm/s at 0.1mm doc, and even at that speed it does not sound good. I’m at a dead end, and the only think left to change is the endmill, but i’ve been using 1/8 carbide 2 flutes which should not be too bad for aluminum.

    sorry the video is out of focus, was focusing on getting ready to e-stop the machine! I the video I am using trochoidal at 10mm/s and 3% step length, with a 3.18 doc

    this is pic of the cut in the video

    .jpg”]

    This is a cut i did on my little dremel 100, for some reason it turned out great

    .jpg”]

    #94441

    Ryan
    Keymaster

    How about a picture of your settings and endmill.

    I use a single flute you can see my settings in the most recent aluminum video. At this point I can say it seems to be spinning really fast, and taking a tiny cut, what happens is you are actually hardening the material by rubbing it not cutting it, that is why I use a single flute (half the speed more room for chip clearing and I turn down the RPM a bit).

    #94444

    Ty
    Participant

    ive tried various different rpm ranges, anything lower than 50% power bogs it down too much, here is a pic of my settings and the endmill, after the cut.

    #94448

    Ryan
    Keymaster

    Have you seen my aluminum video?

    You are trying to cut 3.2mm deep at 15mm/s, and you are trying to plunge at almost max speed. You really have a 3mm diameter bit in a dewalt 660?

    1 user thanked author for this post.
    #94449

    Ryan
    Keymaster

    Settings in the description and the video

    #94472

    Ty
    Participant

    Have you seen my aluminum video?

    You are trying to cut 3.2mm deep at 15mm/s, and you are trying to plunge at almost max speed. You really have a 3mm diameter bit in a dewalt 660?

    Yeah, but that’s with trochoidal on with only a 3% step length. As for the bit size, its 1/8″ i just had to put it to 3.00mm to get my cut dimensions more accurate, things were coming out a bit big. I’m starting to think I need a single flute mill, as its the only thing i’ve not tried yet. So far i’ve noticed on almost every aluminum cut, my chips are really short, even if i’m cutting at 3mm doc with trochoidal the chips are only like 1mm long? when i look at your video the chips look the height of your doc.

    #94486

    Ryan
    Keymaster

    That is still too fast, use my numbers and adjust the trichodial step length only. If your dimensions are off that far something else is wrong as well. Do your cuts and make sure to use a finishing pass.

    Or try it without trichodial and see where it gets you.

    2 users thanked author for this post.
    Ty, Ulli
    #94490

    Eric H
    Participant

    There are a couple of things that might possibly help.

    1. 3% trochoidal step over is pretty low. It seems counterintuitive, but I think you might have some better results if you increase the step-over to 5-10%. This way you will be cutting chips rather than rubbing or melting. You may need to adjust the DOC or feedrate a little if you experience deflection or chatter (1-2mm DOC and 10mm/s should be a good starting place).
    2. Improve chip removal. It looks like you are recutting chips, which will hold all the heat in and welds them to your cutter.
      1. If you can get some type of air blast going it will really help (I use a cheap aquarium pump and it has no problem moving aluminum chips).
      2. The oil may actually be hurting you in this regard, especially if it is pretty viscous, because it will just keep your chips stuck in place. A light coating of WD-40 on your part will lubricate pretty well without gluing chips down.
      3. Increase the slot width. 50% is the norm, but going a little wider will help with chip clearance (at the cost of some extra material and time).

    If you are having issues with oversized parts it is probably deflection. I would recommend adding some light finishing passes or even a “spring pass” instead of “resizing” your endmill. Adjusting the “size” of your tool may compensate for deflection, but you are going to get inconsistent tolerances depending on the material you are cutting.

    Edit: Didn’t see that last post, hopefully this isn’t too redundant.

    1 user thanked author for this post.
    Ty
    #94513

    Ulli
    Participant

    Just an additional remark from someone who just collected some experience with cutting aluminium on an MPCNC.

    Keep the active, protruding end of the end mill as short as possible. That worked wonders here.

    mpcnc_motormounts_20190314_06

    Don’t use oil to lube the cutter. For aluminium, plain ethanol is best. It cools and lubricates. There are voices though who say don’t use it on VHM tools since the thermal shock will induce micro fissures in the drill. Seems I had luck in trying that so far.

    And slow down. Everything. Keep your machine as mechanically tight as possible.The power of a Dewalt (or Makita) is not the same as the tiny dremel.

    Not aluminium, just birch-ply (9mm): A special switchbox for my boat. QCAD, Estlcam, MPCNC.

    Switchbox

    2 users thanked author for this post.
    Ty, Ryan
    #94530

    Ty
    Participant

    First off, that’s an impressive box, did that require much finishing, or did it slot together?. I will get the bit farther in the collet and try those settings with wd40, and i’ll report back.

    #94811

    Ty
    Participant

    Hey guys, just got my single flute end mills in today! and boy, what a difference. It seems all of my previous aluminum cutting issues are gone, I can’t believe how bad those 2 flute end mills must have been, because out of a pack of 10 they all had issues with cutting. Got these cheap single flute end mills, and they work great, its actually cutting the aluminum without any weird noise or vibration, so long as i keep the settings dialed back a bit. Thanks for the input guys, Not sure why my end mills were so bad…

     

    Here’s a little cut I did as a test piece, its a 24mm square, and a circle with a id of 12mm.

     

    photo_2019-03-27_20-05-06-2

    1 user thanked author for this post.
    #94816

    Ryan
    Keymaster

    Awesome!

    Oddly enough I could not get steel to work at all until Kevin told me to use a dual flute, I swore he was crazy. I got so pissed and broke so many single flutes I actually tried it and it worked perfect. Seems very counter intuitive to me but it worked.

    #94820

    Ty
    Participant

    That is interesting, I did try steel with the bits i have, just because I was upset and didn’t care to ruin one of these crappy end mills. For me it just turned out to scream and cause the wood to burn and sparks to fly. I know you and others have stressed it before, but the proper end mill does really make a huge difference. I’m super new to cnc machining, there is a lot to learn, and I’m sure this will not be my last troubleshooting post (><)

     

     

Viewing 13 posts - 1 through 13 (of 13 total)

You must be logged in to reply to this topic.