Results 1 to 4 of 4

Thread: Depth Calculator - Chamfer a hole

  1. #1
    Registered
    Join Date
    Oct 2009
    Location
    USA
    Posts
    77
    Downloads
    0
    Uploads
    0

    Default Depth Calculator - Chamfer a hole

    I am trying create a chamfer on a 3/8 diameter hole. I will first spot drill and then drill to my depth... However, what is the depth value I should enter in the depth value when using the drilling toolpath for the spot drill.

    Does the same thing apply when using a 90 degree countersink ?

    Similar Threads:


  2. #2

    Default

    If I understand you correctly..

    If you have a 90 degree tool and Z0 is top of part, you need to have a Z value of -.1875 for a .375 diameter spot.

    If you want a .005 chamfer, you would need to figure for a .385 diameter (.005+.005+.375) which would be Z-.1925.

    C'sink chart on CNCBasics.com

    So yes, it would be the same as a countersink.

    Mike in MN

    http://www.cncbasics.com
    http://www.cncbasicsforum.com
    http://www.mastercamforum.com
    http://www.mastercamblog.com

    www.cncbasics.com


  3. #3
    Flies Superman's Avatar
    Join Date
    Dec 2008
    Location
    Krypton
    Posts
    1958
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by jcnewbie View Post
    I am trying create a chamfer on a 3/8 diameter hole. I will first spot drill and then drill to my depth... However, what is the depth value I should enter in the depth value when using the drilling toolpath for the spot drill.

    Does the same thing apply when using a 90 degree countersink ?
    It all depends on the type of tool you are using for spotting

    A "spotdrill" assumes the tool shape is to a point, this gives an error in true life as anything more than 1 flute has to have a flat at the point

    so

    Use a "Chamfer tool" to describe your spotdrill, a 1/4" CBD 90° spotdrill may have a "base diameter" of about 0.020", HSS can go as high as 0.050", this should be set accurately

    The parameters to set in a spotdrilling cycle are:-
    Top of stock = top of the hole
    Depth= top of the hole
    --> go into the depth calculator beside "Depth" field, tool angle should be pre-set as 90°, and insert the desired diameter you want and click into another field to show how much deeper you should go, if it is close to what you expect, then "ADD" to depth, Accept, this then is added to the value on the provious page.
    ****caution only add once, or reset the Depth before going in and re-calculating a new diameter****

    When you have set this Chamfer tool correctly, it can be used as a spotdrill and chamfer tool, this eliminates a duplicated tool, toolchange, etc

    NOTE!! as a suggestion have 2 tools in the library, 1 set for spotting or spotchamfering speeds/feeds (ie S2000F6.), and the other for chamfer milling (contouring) S8000F40.



  4. #4
    Registered fizzissist's Avatar
    Join Date
    Apr 2006
    Location
    USA
    Posts
    3197
    Downloads
    0
    Uploads
    0

    Default

    My handy-dandy calculator says that for a given desired dia, for a given tip angle...

    90deg tip, the depth = .5 x desired diameter.
    example you want a .39dia 45deg chamfer, then .5(.39)= .195
    Your Z would be .195 below the surface.

    118deg tip, depth = ~.3 x desired diameter (you can use this for tip allowance if you're too lazy to use Mastercam's tip offset calcuator)

    135deg tip, depth = ~.2 x desired diameter

    ....you need to compensate for the flat at the tip...I fake it, and it's usually close enough



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 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