Page 1 of 2 12 LastLast
Results 1 to 10 of 14

Thread: Chip Load for endmills

  1. #1
    Join Date
    Jan 2005
    Location
    Surrey BC Canada
    Posts
    1,357

    Default Chip Load for endmills

    Where is a good place to get chip load for endmills?
    I have done a couple of Google searches and not come up with a good answer.
    I am trying to figure out some speeds and feeds and I think the load per flute in my CAM software is way out. They have load per flute on a .375 carbide 2 flute EM at at 0.0005. I am wanting to machine some Polycarbonate the the machining time seems really long.
    Thanks
    Dave

  2. #2
    Join Date
    Aug 2006
    Location
    Taylorsville Ky
    Posts
    5,882

    Default

    Why don't you take a piece of the material and start increasing the feed until it starts getting overloaded. Charts are nice but real life is best. It sure won't take many cuts to find out, unless you increase the feed in very small increments.
    It's only ink and paper

  3. #3
    Join Date
    Aug 2009
    Location
    Canada, Bc
    Posts
    7,607

    Default

    yea that sounds like a wonderful chip load if you are trying to melt the polycarb away. :P It should be rather material related. Id think 0.0005 might be for hard steels or finishing pass.. but definately need something higher for polycarb.

    http://www.bmed.mcgill.ca/dept_resou...ill/user_tips/

    Found that googleing for chip load.. has a chart on chip load about half way down.. though it doesnt take material into question...

    Iv seen chip load rates of 0.01~0.02 speced on other sites talking about 10,000rpm brazed/solid carbide router bits through plastics and wood. Likey to help prevent burning at such high RPMs.

  4. #4
    Join Date
    Nov 2005
    Posts
    1,644

    Default

    Chip load varies a lot based on material and the type of tool you're using.

    You either need one of the handbooks, a catalog from the outfit that made your cutter, or one of the handy machinist's calculators.

    Cheers,

    BW
    ---------------------------------------------------

    http://www.cnccookbook.com/index.htm
    Try G-Wizard Machinist's Calculator for free:
    http://www.cnccookbook.com/CCGWizard.html

  5. #5
    Join Date
    Jul 2007
    Location
    No Cal.
    Posts
    1,624

    Default

    Feeds and speeds are typically the best known variables as far as cutting parameters and they are extremely sensitive to minor variations. Unlike many other commonly routed materials, plastics, and particularly acrylics, have an extremely narrow chip load range that can be used to produce an optimal finish (see Figure 7). Each cutter (based on configuration and diameter) will have a different optimum chip load for each material type. As a rule of thumb, the following feed rates are good starting points if the goal is optimum edge finish. A constant spindle speed of 18,000 rpm and a depth of cut equal to the cutter diameter is assumed.

    - 1/8 Diameter Tooling: 75-100 ipm
    - 1/4 Diameter Tooling: 100-200 ipm
    - 3/8 Diameter Tooling: 125 ipm to 250 ipm
    - 1/2 Diameter Tooling: 150 ipm to 300 ipm
    found this

    Of course my machine won't do 18K RPMs but I get pretty good results using carbide tooling @ 4000 rpm & 12 -18 ipm

  6. #6
    Join Date
    May 2007
    Location
    Live Oak, TEXAS
    Posts
    1,512

    Default

    .0005 per flute ?????
    I've never heard of such a wimpy feed rate for carbide endmills.
    For something like polycarbonate, I'd cut at least .010 per flute (.02 per revolution).
    Even when machining Stainless or Inconel, I never drop below .001 per flute.
    Like my old boss used to say: "Crank it up until it breaks, then back off a little!"

  7. #7
    Glacern Guest

    Default

    You can definitely increase your feedrate quite a bit. I haven't machined polycarbonate in a long time, but I feed 3/8" 2-flute endmills through aluminum at .003-.004 IPT.

    Also, depending on your width of cut (WOC), you may be able to increase your feedrate even more due to radial chip thinning. From a top view, chips are crescent shaped, with the maximum chip thickness at the center of the cutter. If your WOC/stepover is less than half the cutter diameter, your actual chip thickness is less than the advance per tooth feedrate (APT, same as IPT).

    To demonstrate this, if you were cutting with a stepover of 20% of the cutter diameter, the maximum chip thickness is 80% of the APT. So the feedrate can be increased by 25% to get the chip thickness back up to the desired level.
    Last edited by Glacern; 09-06-2009 at 08:44 PM.

  8. #8
    Join Date
    Sep 2004
    Location
    Brisbane, CA
    Posts
    442

    Default

    Here's a rule of thumb for a chip load starting point for endmills:

    Chip Load = (EndMill Diameter)/200

    With aluminum that can be pushed up to sometimes twice that chip load for aluminum specific endmill designs. "Hanita" style variable flute carbide endmills for steel can often also go double that chip load.

    But I usually start with the starting point rule of thumb and then adjust feed rate up from there depending on how the machine is taking it.

    For twist drills, replacing the 200 with 100 gets you pretty close.

    I originally saw this "proportional" chip load suggestion in a post by Stan Dornfeld when I was first trying to learn about feed rates, and the method has always worked well for me.

    Paul T.
    Last edited by PaulT; 09-07-2009 at 01:18 PM.

  9. #9
    Join Date
    Aug 2009
    Location
    Canada, Bc
    Posts
    7,607

    Default

    *googles Hanita... googles Hanita varimill*
    PaulT: those varimills look very cool. I wonder why I don't see any in KBC's catalog.. (maybe its because I run in terror from the carbide endmill section after seeing the prices have too many digits) I'll have to keep a mental note about em later when I get into carbide endmills.

    Glacern: Nice to see you arnt just here to sell your wonderful vises. Thats an awsome tip. I have heard about incressing feeds when your doing shallow WOC (width of cut) but I never knew just why you could and how much.

    Just so im understanding the math here, 20% of cutter diamiter, say 1" would be 0.2", or about 40% to the center of the bit. and based on my cheesy inaccuate drawing on a sheet of paper because I don't feel like figureing out the trig or getting out my drafting tools, the tooth exits at about 30degrees before top dead center, cos(30) = 0.86

    So 0.86x chip load is actual chip load, and any speed incress only incresses chip load by the same amount, so you end up with incress in being feed / 0.86 / 0.86 right? say 10IPM to 13.5IPM.

    I can see the incress in feed is much greater with smaller overlaps as the angle quickly gets steeper.

  10. #10
    Join Date
    Jan 2005
    Location
    Surrey BC Canada
    Posts
    1,357

    Default

    Paul,
    Is that per tooth or based on a 2 flute EM?

Posting Permissions

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