584,874 active members*
5,364 visitors online*
Register for free
Login
IndustryArena Forum > Tools / Tooling Technology > CNC Tooling > Breaking bits - Need advise
Results 1 to 5 of 5
  1. #1
    Join Date
    Aug 2013
    Posts
    7

    Breaking bits - Need advise

    I seem to not be using my CNC bits correctly or I had two faulty bits, I'm not quite sure. Either way I need some expert advise for what I should do in order to avoid breaking bits. I'll give you a run down of what I am doing...

    I've had two bits break in the past 3-4 weeks. I purchased two Precise Bits end mill bits (MM208-1250-113FL, 0.1250in dia. 2-flute DeepReach carbide 28.88 57.76 end mill, fish-tail tip, 1.125in DOC, 3in OAL , 1/8in shank). I make 2D kids toys out of poplar wood. I make about 200 different ones. You can see my work at Handmade Wooden Toys - Wood Toys - Waldorf Toys - Kids Toys. The bits were recommended to me by Precise Bits over the phone before I ordered them after I explained to them what I would be using my CNC machine for.

    The only cutting I am doing is 2D profile cutting. The wood I am using is .8125 inch thick poplar. I am cutting in two profile cuts. The first profile cutting depth is .9 inch, with .1 inch passes (so 9 passes for the profile), and with an "allowance offset" of .05 inch and .2 inch thick & .2 inch wide tabs evenly placed around the cutouts. The first profile feed rate is 25 ipm with a plunge rate of 10 ipm. The second profile cutting depth is .9 inch with a single .9 inch pass, with an allowance offset of 0.0, and with .2 inch thick & .2 inch wide tabs evenly placed around the cutouts. The second profile feed rate is 10 ipm with a plunge rate of 5 ipm. The second profile basically shaves the sides of the cut outs to remove the 9 lines left in the side of the cut outs from the first profile cut passes. For all of my cutting I am using "climb" cutting. My router is a DeWalt DWP 611 (16,000-27,000 rpm with adjustable speed) and it runs on setting "5" (speed is controlled in numbers of 1-6) when I am cutting, which I am guessing is around 22500 rpm.

    I have ordered two more MM208-1250-113FL bits that are scheduled to arrive to me tomorrow (9/26). Before I begin cutting more stock I would like to resolve this issue as I am now increasing the amount of cutting I am doing with my CNC and I don't want to be breaking a bit once a week. What am I doing wrong? Am I using the right bits? Should I adjust the feed rates or plunge rates? Perhaps .1 inch is to deep for the passes? Is .05 inch too much to be shaving off the sides of the cut outs in one .9 inch deep pass? I'm just not sure what to adjust and need some expert advise.

    Thank you very much for any and all help!!!

    Dustin

  2. #2
    Join Date
    Dec 2004
    Posts
    783
    I would start with leaving less than .05 to clean off of the profile in one pass, leave just enough that the finish pass gets rid of the tool marks, which if your machine is fairly rigid and trammed to some degree of accuracy shouldn't be much.

    Also look for cheaper bits, precisebits are very nice, I use a few types for certain purposes, but 99%of what I use comes from kyocera http://pages.ebay.com/link/?nav=item...d=380530584040

    That said I would seriously consider using a larger bit http://pages.ebay.com/link/?nav=item...d=380631214319 and maybe use the 1/8" only where needed. Your asking a lot from that bit, breaking one a week from heavy use in poplar might be somewhat normal.

    Sent from tapatalk

  3. #3
    Join Date
    Aug 2013
    Posts
    7
    Thanks for the reply! I use a Probotix V90 that I bolted together myself. I did the anti-backlash nut upgrade and did the 3 axis probostep motor upgrade with a 40V power supply. I took my time bolting it all together and tried to get it as close as I could to having it all right. It was my first time putting a CNC together though.

    When I broke the last bit it was actually while doing the finishing profile pass clean up. Going less than .05 offset might be good. What would you recommend or would you just experiment with it?

    Thank you very much for the links to the cheaper bits! I mainly went with the Precise Bits because I couldn't find anyone else that made a 1/8" bit with at least a 1" DOC. The reason I like the 1/8 is for some of the precision needed for the details on some of the toys I make. Like being able to make the fine points on this princess's crown... (Purple Princess Toy - Fantasy Toy - Figure Toy - Waldorf Toy - Handmade Toy) or being able to get between the leg and bottom of the tail on this fall fox... (Cool Weather Fox Toy - Autumn Toy - Fall Toy - Handmade Wooden Toy). About 1/2 to 3/4 of the toys I make have tight details like that. I think a 1/4" bit would make everything too rounded. I am however tempted to try the 1/8" kyocera that you sent me the link to. It has the right DOC too. I wonder how the 3 flute ball end would work compared to the 2 flute fish tail end bit that I use now from Precise Bits?

    Thanks again,

    Dustin

  4. #4
    Join Date
    Dec 2004
    Posts
    783
    I linked to a 3/16" bit too, from the looks of it you wouldn't lose too much detail, or a quick swipe with a file or folded over sandpaper will give you the detail on the edge, and add some depth to the character.

    Could also experiment with drilling a 1/8" hole in the corners, followed by a profile with the 3/16" bit. Might leave small nubs that could be cleaned up quick with a sharp knife.

    How bad are the steps on the edges in the roughing pass? Are they worse along a certain axis or side of the parts? Tramming the router will help, a tram gauge is not hard to make, dial indicators are cheap enough.

    The ball mill isn't ideal, but should work fine in wood. You will have to plunge a bit deeper to get a flat edge at the bottom is all.

    Since your using such long bits, you might be able to put collars on them as a depth stop, so you won't have to zero the Z when swapping bits, if that's a thought against doing a tool change.

    Sent from tapatalk

  5. #5
    Join Date
    Mar 2003
    Posts
    35538
    I'd ask precise bits for their opinion.
    I'd also try to find a bit with a 7/8" cut length, which will be stronger.
    I'd up the feedrate to at least 100ipm on the first passes if possible. You should be able to cut at 250ipm with 22,000 rpm with no trouble, although the bit is on the long side, so I might reduce the depth of cut a little.
    And, I'd also reduce the finishing pass to about .01".
    Gerry

    UCCNC 2017 Screenset
    http://www.thecncwoodworker.com/2017.html

    Mach3 2010 Screenset
    http://www.thecncwoodworker.com/2010.html

    JointCAM - CNC Dovetails & Box Joints
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

Similar Threads

  1. Breaking Bits
    By Ed_R in forum Material Machining Solutions
    Replies: 7
    Last Post: 05-28-2013, 03:13 AM
  2. Breaking end mills, need advise
    By BNX in forum Tormach Personal CNC Mill
    Replies: 31
    Last Post: 02-24-2013, 01:54 PM
  3. Breaking bits
    By Ansen in forum Glass, Plastic and Stone
    Replies: 0
    Last Post: 10-10-2012, 10:44 PM
  4. i keep on breaking bits???
    By joeyboy in forum Uncategorised MetalWorking Machines
    Replies: 11
    Last Post: 03-24-2004, 10:18 AM
  5. i keep on breaking bits???
    By joeyboy in forum Community Club House
    Replies: 0
    Last Post: 03-23-2004, 01:47 AM

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
  •