please help with radius program
Close
Login to Your Account
Likes Likes:  0
Results 1 to 8 of 8
  1. #1
    Join Date
    Jan 2020
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default please help with radius program

    Could anyone please help me. I need to program a .141 radius into the face of a part on a haas st10. No Y axis or live tooling. Im using a .125 wide full radius groove insert in a holder that points directly into the face of the part.Im not using tool nose comp or anything fancy. Just line for line programming. I don't have much lathe programming experience. Just have to make 6 parts from 316ss. I know the inside dia of the radius starts at x.185 and out from there I guess .282 to make the .141 rad. Please help me! Any help would be much appreciated. Ive never generated a radius like that.

  2. #2
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,241
    Post Thanks / Like
    Likes (Given)
    4758
    Likes (Received)
    1635

    Default

    You're probably gunna have to put up a sketch of what you're doing so folks can have a look see. When cutting on the face depending on the depth and diameter you're cutting the radial clearance on top and bottom of the insert is more of a factor than anything. This is a top notch style insert?

    Brent

  3. #3
    Join Date
    Jan 2020
    Country
    UNITED STATES
    State/Province
    Kentucky
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by ohiomachiner View Post
    Ive never generated a radius like that.
    G01 X(startpoint) z(startpoint)
    G02 X(endpoint of rad) Z(endpoint of rad) R0.141

    The G02 code is a clockwise radius. If you want your tool path to be counterclockwise, use G03 instead. You have to use a little common sense to figure your start and end points. Just make sure the distance between the start z and end z are 0.141. The actual distance between the two x’s should be 0.141 too, but the value would be double if your X axis is diametrical.

    If your tool is 1/8” wide you could do it in two passes G02 and G03 and have the passes meet in the middle. It could be done a few different ways. If the radius is critical you need to be using rad comp.

  4. #4
    Join Date
    Apr 2018
    Country
    UNITED KINGDOM
    Posts
    2,914
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1352

    Default

    Please toss up at least a napkin sketch of what you are trying to do ...

  5. #5
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,674
    Post Thanks / Like
    Likes (Given)
    1238
    Likes (Received)
    2618

    Default

    If you touch your Tool off on the inside of X. Start at
    G0X.177; (.185-.016)
    G1 Z0;
    G2 X.209 Z0. R.016; (.177+.032)
    G1 Z..

    This probably won't throw an Alarm, but it also won't generate ideal results. Hopefully you get the most basic principle.

    R

  6. #6
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,763
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1480

    Default

    Quote Originally Posted by litlerob1 View Post
    If you touch your Tool off on the inside of X. Start at
    G0X.177; (.185-.016)
    G1 Z0;
    G2 X.209 Z0. R.016; (.177+.032)
    G1 Z..

    This probably won't throw an Alarm, but it also won't generate ideal results. Hopefully you get the most basic principle.

    R
    Hello Rob,
    Belated best wishes for the New Year.

    Maybe I'm not seeing the OP's part feature as I should, but how do you get the R0.016 Radius. I'm assuming a concave feature of 0.141rad. With a 0.125 wide, full radius tool, the R would be 0.141 - 0.125/2 = 0.0785.

    With the tool set as a Type 2 tool (typical boring bar setup) and a 0.141 radius face groove having a small diameter of X0.185, I get the following. The finish pass shows the true positions of the tool.

    Regards,

    Bill

    141rad1.jpg

    (0.0625 RADIUS FACE GROOVING TOOL)
    (ROUGH CUTS START HERE)
    G00 X0.5920 Z0.1250
    G01 Z-0.1310
    G04 X0.1
    G01 Z0.0100
    (SEMI FINISH CUT STARTS HERE)
    G01 X0.7290
    G01 X0.7290 Z-0.0625
    G03 X0.4550 I-0.0685 K0.0000 (or G03 X0.4550 R0.0685)
    G01 Z0.0100
    (FINISH CUT STARTS HERE)
    G01 X0.7490
    G01 Z-0.0625
    G03 X0.4350 I-0.0785 K0.0000 (or G03 X0.4350 R0.0785)
    G01 Z0.1250

  7. #7
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,674
    Post Thanks / Like
    Likes (Given)
    1238
    Likes (Received)
    2618

    Default

    Quote Originally Posted by angelw View Post
    Hello Rob,
    Belated best wishes for the New Year.

    Maybe I'm not seeing the OP's part feature as I should, but how do you get the R0.016 Radius. I'm assuming a concave feature of 0.141rad. With a 0.125 wide, full radius tool, the R would be 0.141 - 0.125/2 = 0.0785.

    Bill, I'd been waiting a long time for this. I thought you were wrong, but I was mistaken.

    R

    .141 is a radius not a diameter.

  8. #8
    Join Date
    Jan 2020
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Thanks for the help. I appreciate it. got it done using a g42 and tip 7.....


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
  •