turn an ellipse

Results 1 to 8 of 8

Thread: turn an ellipse

  1. #1
    Registered Ivanowitsch's Avatar
    Join Date
    Oct 2010
    Location
    Hittnau
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default

    Hello everybody,
    I want to turn an ellipse on our EMCO E45 lathe. (each with an inner and outer contour)

    Does anybody know if that’s possible and it is how it’s been done?
    Many thanks and greetings
    Ivan



  2. #2
    Registered reitstock's Avatar
    Join Date
    Dec 2006
    Location
    Allg
    Posts
    83
    Downloads
    0
    Uploads
    0

    Default

    Hello,

    You can do almost everything with the machine and the controller. However without a drawing or sketch it’s difficult.
    Greetings from the mountains.



  3. #3
    Registered Ivanowitsch's Avatar
    Join Date
    Oct 2010
    Location
    Hittnau
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default

    here are the sketches for the inner and outer contour...

    [attachment=8629:ellipse_aussen.JPG]
    [attachment=8630:ellipse_innen.JPG]



  4. #4
    CNCFr's Avatar
    Join Date
    Sep 2002
    Location
    Timbuktu
    Posts
    1950
    Downloads
    0
    Uploads
    0

    Default

    I would try it like this:

    Set the neutral point to the centre of the ellipse (trans….)
    Trans….
    ASCALE Z=40.054 / 23.5
    g1 z0 x23.5
    g2 z21.708 x9 i-23.5

    And in the other case
    trans...
    ASCALE Z= 31 / 21
    g1 z0 x21
    g2 z21 x0 i-21

    It’s not tested!



  5. #5
    Registered Ivanowitsch's Avatar
    Join Date
    Oct 2010
    Location
    Hittnau
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default

    I tried but I get the following error description:

    14040 channel 1 Set endpoint of circle error
    The cursor stands then on the set: G1 Z0 X23.5

    coangry.gif



  6. #6
    CNCFr's Avatar
    Join Date
    Sep 2002
    Location
    Timbuktu
    Posts
    1950
    Downloads
    0
    Uploads
    0

    Default

    I tried but I get the following error description:

    14040 channel 1 Set endpoint of circle error
    The cursor stands then on the set: G1 Z0 X23.5

    coangry.gif

    Possible causes for the error could be:
    G18 is not activated ( I counted on G18 to be activated)
    The diameter programming is active (DIAMON instead of DIAMAOF)

    Another possibility: the controller has a bigger resolution than 3 ractional digits .
    Then you have to enter Z more detailed. Instead of 21.708 it’s then 21.70829335...

    I tried it out with my machine and it worked....



  7. #7
    Registered Ivanowitsch's Avatar
    Join Date
    Oct 2010
    Location
    Hittnau
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default

    I had to enter DIAMOF. Thanks a lot!
    How does your program looks like? I never done ISO programming on the EMCO, only via Shopturn.
    Mine looks like this:

    ;_N_1001_MPF
    G0 G53 X280 Z250 D0
    G96 S200
    DIAMOF
    T2 D1 M6
    G0 G42 X-1.5 Z1 M3
    G1 X0 Z0 F0.2 M8
    TRANS X0 Z0
    ASCALE Z=40.054 / 23.5
    G1 Z0 X23.5
    G3 Z-21.708 X9 I-23.5
    M30

    And another question: why is the Z value 21.708? Endpoint is on 37?



  8. #8
    CNCFr's Avatar
    Join Date
    Sep 2002
    Location
    Timbuktu
    Posts
    1950
    Downloads
    0
    Uploads
    0

    Default

    And another question: why is the Z value 21.708? Endpoint is on 37?
    I calculated it like the following method:
    The basic form of a circle with the radius 23.5, that ends at X9.
    Then is Z= SQRT(23.5 * 23.5 - 9 *9)) = 21.708

    This circle is then stretched on the Z axle by the factor 40.054 / 23.5.
    Then you arrive at the endpoint that is 37.
    You could have calculated the Z end point of the circle also like this:
    37 * 23.5 / 40.054 = 21.708



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 for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

turn an ellipse

turn an ellipse