wobbling problems - Page 2


Page 2 of 2 FirstFirst 12
Results 21 to 22 of 22

Thread: wobbling problems

  1. #21
    Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5516
    Downloads
    0
    Uploads
    0

    Default Re: wobbling problems

    Quote Originally Posted by ellobo91 View Post
    Also, maybe a bit off-topic though, do you have any tips on where I could read/learn some basics on feedrates, spindle speeds, behaviour of materials and cutters etc. Better to read some basics and come back here a bit better educated than to post more stupid questions than needed. Have heard some here about if i decrease stepover I need to increase feedrate? In my ignorance i thought the lower, the better (on both stepover and feedrate)
    In theory, you would take the CHIPLOAD recommended by the tool manufacturer, and multiply that by the number of flutes on the tool and spindle RPM, and that will give you the theoretical feedrate, in IPM. In practice, most DIY machines can't push these tools the way a VMC can, so you'll have to derate the stepover, or depth of cut, to get a clean cut. You'll have to do this by trial and error on your machine, meaning be ready to break some bits. Once you find the optimal federate and RPM, you can work backwards to see exactly what chipload you actually have, then you can base your other tools on these numbers. But the basic thing is, if you find your 1/4" tool has a chipload of .002" per tooth (which is probably a good place to start), then for a 1/8" tool you can expect to use a chipload of .001" and for a 1/2" tool .004". In other words the federate would be proportional to the tool size, at least for pocketing and profiling.

    What you're referring to is more related to the material removal rate. Once you have your parameters dialed in, you can figure out what your MMR is. Which is your depth of cut (aDoC) times the width of cut (rDoC or stepover) times the federate. You don't want to venture too far from this number, but you find you have the same MMR whether you twice as deep but half as fast as normal, or twice as fast or half as deep. Once you figure out which way your machine works best (and for most routers it's more toward the former) then you can tweak the depths and stepovers.

    __________________________________________________ __


    I should add, don't just rely on friction between your frame members to keep things together. The joints will work themselves loose over time from vibrations and such. Gussets, pins, pockets, etc. that provide a mechanical means of preventing movement goes a long way to stiffen up a machine.



  2. #22
    Member
    Join Date
    Jun 2011
    Location
    US
    Posts
    692
    Downloads
    0
    Uploads
    0

    Default Re: wobbling problems

    re: increasing feedrate when decreasing stepover. When your stepover gets very small (less than 10% the tool diameter or so,) chip thinning starts to really come into play. I'm not going to explain it here, but John @ NYC CNC does a pretty good job of it
    (he's got a lot of decently useful videos and I find them to be fairly entertaining as well.)
    For a machine as light as yours, you want to be using the minimum chip load a tool will tolerate as well as narrow stepovers and shallow DOC. Most good 1/4" carbide can tolerate down to .001" chip load, really probably half that. It's probably not a bad starting point at a narrow stepover though. I'd try a 2-flute, short as you can find 1/4" and 1/8" carbide flat end mills. Chuck them up in the collet until the flutes are almost in the collet. Run 12k RPM for the 1/4", 24k for the 1/8", .03 stepover and depth for the 1/4" and .015 stepover, .03 depth for the 1/8" and around 24 IPM for both.
    Try these on straight cuts on the edge of a work piece. Once you have cut a little, start adjusting parameters, one at a time and take notes. Don't be afraid to increase parameters, sometimes things go better a bit harder.
    I'd also try conventional milling as well as climb milling. I'd guess climb will work better for you, as it's a bit more forgiving of lacking rigidity, conventional is more forgiving of backlash/slop.



Page 2 of 2 FirstFirst 12

Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

wobbling problems

wobbling problems