Results 1 to 4 of 4

Thread: Ball Mill

  1. #1
    Registered
    Join Date
    Feb 2010
    Location
    united states
    Posts
    9
    Downloads
    0
    Uploads
    0

    Ball Mill

    I am new to running and programming a Citizen L20 swiss screw machine. I am going to be machining a handle made out of tit. After a long radius is turned using a G3 code, is it possible to go over the same radius at a shallower depth with a ball end mill? I need to put a shallow line at 90^ increments. The line actually starts out shallow and gets deeper in the center then gets shallower again. Can a G3 code be used for an endmill the same way it is used for a turning tool? Thanks for your help!!


  2. #2
    Registered
    Join Date
    Oct 2008
    Location
    UK
    Posts
    31
    Downloads
    0
    Uploads
    0
    "Can a G3 code be used for an endmill the same way it is used for a turning tool?"

    Yes - All you have to do is change the plane selection before milling e.g

    M5 G98
    M58 S3=2000
    T700
    M18 C0
    G50 W-0.59
    G0 X* Z* Y* T*

    G19 - Plane select for Y and Z

    G3 Y* Z* R* F*
    G1 Y*

    G0 X* T0

    G18 - Std Plane select for X and Z

    G50 W0.59
    M20 M60 G99

    If you want to "wrap" milling tool round bar you'll need G12.1/G16 plane and any Y axis moves become C and values are radiall

    E.g

    M5 G98
    M58 S3=2000
    T700
    M18 C0
    G50 W-0.59
    G0 X* Y* Z* T*
    G1 X* F*
    G12.1
    G16 C*

    G3 Z* C* R*
    G1 Z*
    G0 X*
    G13.1
    G18
    G0 X* T0
    G50 W0.59
    M20 M60 G99


    Good luck


  3. #3
    Registered
    Join Date
    Feb 2010
    Location
    united states
    Posts
    9
    Downloads
    0
    Uploads
    0

    Wink Ball Mill

    UK-Engineer:
    Thanks for your help. I am not making the part at this moment, just needed to know if it was possible. Thanks again!


  4. #4
    Registered
    Join Date
    Mar 2008
    Location
    USA
    Posts
    432
    Downloads
    0
    Uploads
    0
    UK-Engineer,

    Are you sure about needing to change the interpolating plane for this? It seems to me that the turning operation is already done in G18 X-Z mode. No? Since the L-series has live tools rotating 90º to the workpiece, as the gang tools are also oriented, the G19 Z-Y mode would be for use if using a t-slot type of cutter in the "side" of the work. This is a ball mill, presumably using the tip.

    The only difference is that the machine stops the spindle, lights up the live tool spindle and moves (in most cases) in the "G98" mode instead of "G99". Maier CNC screw machines can use live tools in either mode.


Similar Threads

  1. Ball end mill help
    By foamcutter in forum General Metalwork Discussion
    Replies: 4
    Last Post: 07-21-2010, 01:59 PM
  2. 1/8 ball mill longest cut?
    By 1ctoolfool in forum Haas Mills
    Replies: 6
    Last Post: 03-11-2008, 11:40 PM
  3. special ball end mill
    By 98vert in forum Metal Working Tooling
    Replies: 3
    Last Post: 12-14-2006, 04:35 PM
  4. Stepover and ball/end mill
    By Sanghera in forum DIY CNC Router Table Machines
    Replies: 9
    Last Post: 08-01-2006, 10:54 PM
  5. Ball Screws For Jet Mill
    By michaeljt in forum Linear and Rotary Motion
    Replies: 4
    Last Post: 06-30-2005, 01:32 PM

Posting Permissions


 


About CNCzone.com

    We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed


Search Engine Friendly URLs by vBSEO ©2011, Crawlability, Inc.