Fanuc 15-M ignoring circular lines of code


Results 1 to 5 of 5

Thread: Fanuc 15-M ignoring circular lines of code

  1. #1
    Member Moog199's Avatar
    Join Date
    Apr 2020
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Fanuc 15-M ignoring circular lines of code

    I ran a program on the 3 axis mill and the Fanuc 15-m is ignoring the G03 line in some instances but not others.
    About 40 holes were cut and with 4 holes the m/c ignored the circular move all together, I ran it through a few times on single block, watched as it read the circular move but totally ignored it.

    G40 G94 G17 G80 G21 G49
    ( TP NAME= CHAM-3 )
    ( T0 )
    ( T NAME=CHAMFER TOOL DIA= 3.000 LENGTH= 75.000 )
    M0
    M8
    G0 G90 X2.05 Y-24.986 S2000 M3
    Z25.
    Z3.
    G1 Z-1.5 F280. D0
    X3.55
    G3 Y-24.987 I-3.55 J0.0
    G1 X2.05 Y-24.986
    Z3.
    G0 Z25.
    X-36.207 Y-86.496
    Z3.
    G1 Z-1.5
    X-37.707
    G3 Y-86.497 I1.55 J0.0
    G1 X-36.207 Y-86.496
    Z3.
    G0 Z25.
    X-56.257
    Z3.
    G1 Z-1.5
    X-57.757
    G3 Y-86.497 I1.55 J0.0
    G1 X-56.257 Y-86.496
    Z3.
    G0 Z25.
    M9
    G91 G28 Z0.0
    G91 G28 X0.0 Y0.0
    (M61-----OR----M62 INSERT HERE)
    (MACHINE RUN-TIME = 0hrs 0min 15sec)
    M30
    %

    I've spliced out the problem lines to test again in a small test program, It performs the first G03 line but ignores the second 2.

    I looked at the rest of the holes in the big program, and many holes are the same format (software generated)
    How can the m/c just ignore it, surely if it didn't like the code it would throw an error, not just carry on as if it wasn't there.

    I managed to get these problem holes cut, by re-selecting them in the software differently, until the start move it selected went along a different quadrant direction, then finally the m/c cut those holes.
    The issue is, I don't see a problem with the code, so why is it doing it?

    Similar Threads:


  2. #2
    Member
    Join Date
    May 2016
    Location
    United States
    Posts
    279
    Downloads
    0
    Uploads
    0

    Default Re: Fanuc 15-M ignoring circular lines of code

    I back plotted your code and the 2nd and 3rd G3's do not create circles like the first does but just a short line. Meaning the code is messed up. If the three holes here are all the same size and supposed to be done in the same manner , then here's what I got when moving to the 2nd hole position coordinate and pasting the back plotted hole 1 tool path to it and then creating code from that.

    G1Z-18.923
    X37.707
    G3Y-86.497I-3.55J0.

    This is different then yours.

    Anyway... the short story is the code is messed up. Maybe copy and past the hole that works into the location of the two that don't and try again.



  3. #3
    Member Moog199's Avatar
    Join Date
    Apr 2020
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default Re: Fanuc 15-M ignoring circular lines of code

    thanks for your help, that's a worry that the software output dodgy code, I'll look at the post processor maybe run the program through another generic one, and see if the same error occurs



  4. #4
    Member lucaswalker's Avatar
    Join Date
    Sep 2018
    Posts
    9
    Downloads
    0
    Uploads
    0

    Default Re: Fanuc 15-M ignoring circular lines of code

    Hi,

    The NC is acceptable yet not perfect,

    All the G3 are supposed to generate a complete 360° circular move, so the end point should be at the same coordinates that the start point, and IJ gives the center.
    If we look at the the second G3 we start at X=-37.707, Y=-86.496 and we got to X="" (so the same X) and Y=-86.497
    Because of the 1/100 mm of difference between the start and the end, the control perform a very small arc move rather than the complete circle.
    The tolerance on this behaviour can usually be managed with some parameters within the controller.

    A part from that a more correct NC would not print X or Y on the G3 moves, so we can be sure that the start and end point are the same which will force the controller to perform the full circle. It should go like this:

    G40 G94 G17 G80 G21 G49
    ( TP NAME= CHAM-3 )
    ( T0 )
    ( T NAME=CHAMFER TOOL DIA= 3.000 LENGTH= 75.000 )
    M0
    M8
    G0 G90 X2.05 Y-24.986 S2000 M3
    Z25.
    Z3.
    G1 Z-1.5 F280. D0
    X3.55
    G3 I-3.55 J0.0
    G1 X2.05 Y-24.986
    Z3.
    G0 Z25.
    X-36.207 Y-86.496
    Z3.
    G1 Z-1.5
    X-37.707
    G3 I1.55 J0.0
    G1 X-36.207 Y-86.496
    Z3.
    G0 Z25.
    X-56.257
    Z3.
    G1 Z-1.5
    X-57.757
    G3 I1.55 J0.0
    G1 X-56.257 Y-86.497
    Z3.
    G0 Z25.
    M9
    G91 G28 Z0.0
    G91 G28 X0.0 Y0.0
    (M61-----OR----M62 INSERT HERE)
    (MACHINE RUN-TIME = 0hrs 0min 15sec)
    M30
    %



  5. #5
    Member
    Join Date
    May 2016
    Location
    United States
    Posts
    279
    Downloads
    0
    Uploads
    0

    Default Re: Fanuc 15-M ignoring circular lines of code

    Yes changing the Y86.497's to 86.496 fixed it. The 2nd and 3rd holes are smaller then the first as well. I work in inches most the time and my software and machine will most times let a 0.0001" thing pass if I'm not mistaken.

    I noticed that discrepancy when first looking it over but didn't take it to be enough to matter. I also think you're right that the tolerance band can be adjusted via parameter.

    Nice call lucaswalker.



Tags for this Thread

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

Fanuc 15-M ignoring circular lines of code

Fanuc 15-M ignoring circular lines of code

Fanuc 15-M ignoring circular lines of code