Results 1 to 10 of 10

Thread: Chamfering question

  1. #1
    Registered
    Join Date
    Apr 2005
    Location
    USA
    Posts
    40
    Downloads
    0
    Uploads
    0

    Chamfering question

    Hello, lets say I have a plate with a 0.75" hole in it. I want to put a small chamfer on the top (inside) of the hole just to break the edge, so I don't have to do it by hand. So I go into Mastercam X4, select circle mill, set up my 90° 0.5" chamfer mill. Is there a way to set up my offsets for the chamfer mill, so I am not using just the tip of the tool? I want to use something like 2D Chamfer, but everytime I use 2D CMFR, the tool always starts on the outside of the hole, instead of the inside, is there a better way? I am new to Mastercam, thanks.


  2. #2
    Registered
    Join Date
    Dec 2009
    Location
    Sweden
    Posts
    79
    Downloads
    0
    Uploads
    0
    Hi, click on the geometry tab of the operation, right-click on the chain and then select "change side". Regenerate and the tool will cut inside of your circle.


  3. #3
    Registered
    Join Date
    Apr 2005
    Location
    USA
    Posts
    40
    Downloads
    0
    Uploads
    0
    Thank you, that helped for the start of the tool. However now it says that the tool is too small to create the chamfer. I am using a 12 mm chamfer tool, with a .039" diameter flat on the bottom of the insert, and a .472" diameter on the diameter of the whole insert. In the 2D chamfer I am using .1" for the width, and 0.0 for the tip offset, so I can use the side of the insert instead of the tip so it doesn't leave a flat on the chamfer. The tool diameter in the tool page I am using .039 for the flat. If I use .472 (12mm) it creates too large of a chamfer. My Z depth in the Linking parameters is 0.0. I am not sure what to do next.


  4. #4
    Registered
    Join Date
    Aug 2008
    Location
    USA
    Posts
    64
    Downloads
    0
    Uploads
    0
    Forget the "Circle Mill" and just use "Contour". Then, since your angle is 45^, offset the edge you want to chamfer. Go equal amounts over and down. If you offset a 1/4" your cut depth will be 1/4".


  • #5
    Registered
    Join Date
    Dec 2009
    Location
    Sweden
    Posts
    79
    Downloads
    0
    Uploads
    0
    If you zip and upload your .mcx file I can have a look at the parameters.


  • #6
    Registered
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    41
    Downloads
    0
    Uploads
    0
    Quote Originally Posted by utengineer04 View Post
    Thank you, that helped for the start of the tool. However now it says that the tool is too small to create the chamfer. I am using a 12 mm chamfer tool, with a .039" diameter flat on the bottom of the insert, and a .472" diameter on the diameter of the whole insert. In the 2D chamfer I am using .1" for the width, and 0.0 for the tip offset, so I can use the side of the insert instead of the tip so it doesn't leave a flat on the chamfer. The tool diameter in the tool page I am using .039 for the flat. If I use .472 (12mm) it creates too large of a chamfer. My Z depth in the Linking parameters is 0.0. I am not sure what to do next.
    Is your tool geometry defined correctly in your tool list?

    .1" width is more than 'just breaking the edge'. Use 0.01" as width
    Always add a something to the tip offset unless you are chamfering straight off a flat face. try 0.02"
    For best results always have a lead in bigger than the chamfer you are cutting!

    Hope this helps

    C


  • #7
    Registered Superman's Avatar
    Join Date
    Dec 2008
    Location
    Krypton
    Posts
    1,768
    Downloads
    0
    Uploads
    0
    The guy's are correct, don't use circlemill

    Tool
    Use a chamfermill, set the point diameter and Taper angle very accurately ( these are what are used in the toolpath calculation )
    Op
    use 2D contour
    Top of stock = the TOP face of the chamfer
    Depth = the TOP face of the chamfer
    XY stock to leave = 0
    Z stock to leave = 0
    Contour type = 2D chamfer ( or 3D chamfer- with some restrictions )
    Width = 0.01" ( will give this size chamfer )
    Tip offset = 0.04" ( how far the tip extends below the bottom of the width size ) ( adjust only this to make it cut higher up the flutes )

    Lead in /out
    line perpendicular length = 0.05"
    arc = 0 ( you can try 0.05" )
    arc sweep = 45°

    then, copy LH to RH

    PS
    on profiles, you can lengthen or shorten the path, if near walls etc.

    using the above settings, the tool tip will be passing 0.05" below your "Depth" value setting [0.01"+0.04"])


  • #8
    Registered
    Join Date
    Apr 2005
    Location
    USA
    Posts
    40
    Downloads
    0
    Uploads
    0

    Talking

    Quote Originally Posted by Superman View Post
    The guy's are correct, don't use circlemill

    Tool
    Use a chamfermill, set the point diameter and Taper angle very accurately ( these are what are used in the toolpath calculation )
    Op

    PS
    on profiles, you can lengthen or shorten the path, if near walls etc.

    using the above settings, the tool tip will be passing 0.05" below your "Depth" value setting [0.01"+0.04"])

    Thank you very much, that is what I was wondering, what diameter is used to create the toolpath. Excellent, thanks for everyones help, I appreciate it.


  • #9
    Registered
    Join Date
    Nov 2006
    Location
    US
    Posts
    248
    Downloads
    0
    Uploads
    0
    I've had troubles getting the chamfer operation to perform exactly like I wanted. What I prefer to do instead is define a 45º angled too with an outside diameter of, say, 0.25, tell it to do down half of it so mastercam thinks it's right on the edge. Then, in reality I use a tool with a larger diameter, like 3/8" or more (depending on what the geometry allows). Use CDC with the toolpath and program it as 0.25 in your machine's CDC diameter register. The machine will compensate the tool enough that it doesn't cut in the middle, and doesn't cut on the absolute edge either.

    Basically I call upon the number in the CDC register to determine what will happen on the fly. It can be useful when you have inside edges being chamfered, where you don't have much room to go crazy with large tools.


  • #10
    Registered Mike Mattera's Avatar
    Join Date
    Mar 2006
    Location
    USA
    Posts
    1,011
    Downloads
    0
    Uploads
    0
    Use contour and select 2D Chamfer instead of just 2D.
    Set the amount of chamfer you need (.012).
    Depth will be how much past the bottom of the tool you want.

    It's really very easy. No math required.

    Mike Mattera
    Tips For Manufacturing Training CD's, DVD's for Mastercam, SolidWorks, Inventor, G-Code Training & More
    http://www.tipsforcadcam.com


  • Similar Threads

    1. Chamfering Help Please!!
      By Randy727 in forum Solidworks
      Replies: 3
      Last Post: 07-22-2010, 06:27 PM
    2. Chamfering tool
      By David Da Costa in forum General Metalwork Discussion
      Replies: 3
      Last Post: 08-07-2009, 06:31 PM
    3. Chamfering??
      By BulleTxMagneT in forum Dolphin CADCAM
      Replies: 2
      Last Post: 09-14-2007, 11:47 PM
    4. Need help in chamfering
      By abcdef in forum General Metalwork Discussion
      Replies: 15
      Last Post: 04-24-2007, 07:34 PM
    5. chamfering
      By Mortek in forum General Metal Working Machines
      Replies: 4
      Last Post: 02-06-2004, 10:24 PM

    Visitors found this page by searching for:

    Nobody landed on this page from a search engine, yet!
    SEO Blog

    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.