G72 Cuts more than programed
Close
Login to Your Account
Results 1 to 7 of 7
  1. #1
    Join Date
    Aug 2018
    Country
    UNITED STATES
    State/Province
    Oklahoma
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default G72 Cuts more than programed

    Hey I can't find any one with this problem. I was working on a part and using my Doosan Lynx 220 Turning center. Graphed before running the part. The machine wants to cut .030 more than I programmed.

    M00;
    ;
    ;
    T101;
    G50 S3000;
    G96 S500 M03;
    G00 G54 G42 X2.3 Z0.25;
    M08;
    G72 W0.05 R0.01 (0.05 IS TO SEED UP SIM);
    G72 P05 Q09 U0.0 W0.0 F0.002;
    N05 G01 X2.3 Z0.0;
    Z0.0;
    N09 X-0.033;
    ;
    ;

    The last cut is Z-0.030 when it should be Z0.0
    Many thanks in advanc.

  2. #2
    Join Date
    Feb 2017
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    69
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    27

    Default

    Probably your cutter comp G42. Try it without.


    When i run a G72 it would look like this:
    T101;
    G50 S3000;
    G96 S500 M03;
    G00 G54 G40 X2.3 Z0.25;
    M08;
    G72 W0.05 R0.01 (0.05 IS TO SEED UP SIM);
    G72 P05 Q09 F0.002;
    N05 G0 Z0.0;
    N09 G1 X-0.033;

  3. #3
    Join Date
    Dec 2014
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    1,245
    Post Thanks / Like
    Likes (Given)
    352
    Likes (Received)
    577

    Default

    CAM or fingerCAM? Do you have the TNR, quadrant etc defined properly for TNR comp?

  4. #4
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,458
    Post Thanks / Like
    Likes (Given)
    4048
    Likes (Received)
    2635

    Default

    I'm pretty sure the G42 needs to be in the G72 cycle on the N05 line.
    Even though the G72 doesn't read the G42 INSIDE the P and Q lines, the G70 will. And since you have it turned on before the cycle, that might be where your .03 is coming from... assuming you have .03 in your comp.

  5. #5
    Join Date
    Mar 2003
    Location
    Upstate New York USA
    Posts
    281
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    43

    Default

    why bother using TNRC on a straight line face cut move anyway?

  6. #6
    Join Date
    Aug 2018
    Country
    UNITED STATES
    State/Province
    Oklahoma
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Hazzert, I used FingerCAM and I have tip 3 with a 0.015 R in tool geometry
    Tom the G72 was an after thought. I am still learning G-Code at tech and thought a G71 could handle the whole thing.
    I'll try turning off TNRC.

  7. #7
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,611
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1416

    Default

    Quote Originally Posted by KevinEwards View Post
    Hey I can't find any one with this problem. I was working on a part and using my Doosan Lynx 220 Turning center. Graphed before running the part. The machine wants to cut .030 more than I programmed.

    M00;
    ;
    ;
    T101;
    G50 S3000;
    G96 S500 M03;
    G00 G54 G42 X2.3 Z0.25;
    M08;
    G72 W0.05 R0.01 (0.05 IS TO SEED UP SIM);
    G72 P05 Q09 U0.0 W0.0 F0.002;
    N05 G01 X2.3 Z0.0;
    Z0.0;
    N09 X-0.033;
    ;
    ;

    The last cut is Z-0.030 when it should be Z0.0
    Many thanks in advanc.
    Hello Kevin,

    1. As Tom points out, there is no need whatsoever in using TNR Comp on a Face Cut that is perpendicular to the Z axis.

    2. The tool is to the Left of the Tool Path in the direction it travels, accordingly, G41 should be used, not G42; that is the reason for your over-cut.

    Regards,

    Bill

  8. Likes rainman liked this post

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
  •