Need help with mill programming!
Close
Login to Your Account
Results 1 to 8 of 8
  1. #1
    Join Date
    Jan 2003
    Location
    Imlay City, Michigan
    Posts
    1,713
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    141

    Default Need help with mill programming!

    Hello all,

    I’m stuck, I’m trying to machine a profile at an angle on the top surface of a part?

    I’ve done this in the past and I cannot for the life of me remember what I did? I remember it was something simple, only a couple of lines of code to do what I needed?

    I’ll describe what I’m trying to do the best I can.

    I’m starting from the right hand side of the part and cutting a profile in the G18 plane using a 1/4 ball end mill programmed from the center of the ball.

    Here’s a picture of the profile;

    aa613e13-dbe1-4817-ade8-2de738b33058.jpg

    I programmed an M97 with a loop to machine this profile. I need to be able to shift in X and Y after the profile is cut so I can cut the profile at an angle on the top of the part?

    Problem I’m having is, I can get the Y to shift but not in X, now I’m totally lost!

    Any one have any ideas how to do this?
    I cannot mount the part at angle, I’m machining a pocket between to walls in the part!

    I can post the program tomorrow when I get to work!

    Any help would be appreciated! I tried calling Gerotech who gave me the info in the past, and they have no idea how to do this now?

    Thanks for any help!

    Kevin

  2. #2
    Join Date
    May 2007
    Country
    UNITED STATES
    State/Province
    Massachusetts
    Posts
    795
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    52

    Default

    Hi Kevin,

    Let's see what you have for code this far. Post the part of the program you're having trouble with, and we can point you in the right direction. Teach a guy how to fish.

  3. #3
    Join Date
    Jan 2003
    Location
    Imlay City, Michigan
    Posts
    1,713
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    141

    Default

    Quote Originally Posted by beege View Post
    Hi Kevin,

    Let's see what you have for code this far. Post the part of the program you're having trouble with, and we can point you in the right direction. Teach a guy how to fish.
    Here's the code I have right now.


    %
    O00165

    T17 M06
    G00 G90 G18 G54 X0. Y-0.08
    S6000 M03
    G43 H17 Z1. M08
    G00 Z0.1
    G01 Z0. F300.
    G03 X0.7001 Z-0.4809 R0.75
    G01 X0.862
    G03 X1.5621 Z0. R0.75
    G00 Z1.
    M97 P1000 L85
    G00 G90 Z1.
    M30



    N1000
    G90 G00 Z0.1
    G90 G01 Z0. F300.
    G01 Z0.
    G03 X0.7001 Z-0.4809 R0.75
    G01 X0.862
    G03 X1.5621 Z0. R0.75
    G00 Z1.
    G90 G00 X0.
    G91 G00 Y0.005
    G91 G00 X0.0006
    M99
    %

    This shifts the start point in Y0.005 before each cut, but the X0.0006 line does nothing, I'm stumped!

    Kevin

  4. #4
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    754
    Post Thanks / Like
    Likes (Given)
    425
    Likes (Received)
    743

    Default

    Your profile needs to be in incremental also. Its programmed to go to those absolute X coords every pass regardless of the X shift amount. That's why Y moves OK but X doesn't.
    Also I don't see switch back to G17


    O00165

    T17 M06
    G00 G90 G18 G54 X1.5621 Y-0.08 (position at the end of the profile)
    S6000 M03
    G43 H17 Z1. M08
    G00 Z0.1

    M97 P1000 L85
    G00 G90 Z1.
    M30


    N1000
    G91 G00 X-1.5621 (shift back to beginning of the profile)
    G1 Z-.1
    G03 X0.7001 Z-0.4809 R0.75
    G01 X0.1619
    G03 X.7001 Z.4809 R0.75
    G00 Z.1

    X.006 Y.005

    M99

  5. #5
    Join Date
    May 2007
    Country
    UNITED STATES
    State/Province
    Massachusetts
    Posts
    795
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    52

    Default

    I don't see a G18 anywhere. A G3 in a G18 plane NEEDS a G18. And don't forget to go back to G17 when you're done.

  6. #6
    Join Date
    Jan 2003
    Location
    Imlay City, Michigan
    Posts
    1,713
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    141

    Default

    Quote Originally Posted by Booze Daily View Post
    Your profile needs to be in incremental also. Its programmed to go to those absolute X coords every pass regardless of the X shift amount. That's why Y moves OK but X doesn't.
    Also I don't see switch back to G17


    O00165

    T17 M06
    G00 G90 G18 G54 X1.5621 Y-0.08
    S6000 M03
    G43 H17 Z1. M08
    G00 Z0.1

    M97 P1000 L85
    G00 G90 Z1.
    M30


    N1000
    G91 G00 X-1.5621 (shift back to beginning of the profile)
    G1 Z-.1
    G03 X0.7001 Z-0.4809 R0.75
    G01 X0.1619
    G03 X.7001 Z.4809 R0.75
    G00 Z.1

    X.006 Y.005

    M99
    Quote Originally Posted by beege View Post
    I don't see a G18 anywhere. A G3 in a G18 plane NEEDS a G18. And don't forget to go back to G17 when you're done.
    I have G18 in the main program, do I need it in the sub program as well?

    Kevin

  7. #7
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    754
    Post Thanks / Like
    Likes (Given)
    425
    Likes (Received)
    743

    Default

    No you're fine.

    O00165

    T17 M06
    G00 G90 G18 G54 X1.5621 Y-0.08
    S6000 M03
    G43 H17 Z1. M08
    G00 Z0.1

    M97 P1000 L85
    G00 G90 G17 Z1.
    M30

    I'm not sure if M30 resets everything back to default so it's good practice to program back to XY plane so your next program doesn't do something goofy.

  8. #8
    Join Date
    Jan 2003
    Location
    Imlay City, Michigan
    Posts
    1,713
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    141

    Default

    Here's the updated program and its running fine now!

    %
    O00166

    T18 M06
    G00 G90 G18 G54 X1.5621 Y-0.135
    S6000 M03
    G43 H18 Z1. M08
    G00 Z0.1

    M97 P1000 L300
    G00 G90 Z1.
    M30


    N1000
    G91 G00 X-1.5621 (shift back to beginning of the profile)
    G01 Z-0.1 F150.
    G03 X0.7001 Z-0.4809 R0.75
    G01 X0.1619
    G03 X0.7001 Z0.4809 R0.75
    G00 Z0.1

    X0.0006 Y0.005

    M99
    %


    Thanks everyone for the help!

    Kevin


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  
2