Post Processor for Bobcam Wire FX20 - G54 vs G92?
Close
Login to Your Account
Likes Likes:  0
Results 1 to 10 of 10
  1. #1
    Join Date
    Jun 2016
    Country
    CANADA
    State/Province
    Ontario
    Posts
    38
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Post Processor for Bobcam Wire FX20 - G54 vs G92?

    I purchased Bobcam wire and it has gone from them telling me they can modify a post processor in a couple weeks, into they can look at it 6-8 week after a month has passed (not pleased). Anyway now I have to modify and change the post on my own. It's not terribly difficult and if anyone has one for a Mitsubishi FX20 that would be great. But one thing I'm trying to understand is what benefits or differences are there to use G92 or G54 in programming for part setup to adjust the post accordingly.

    I had a test program with G92 and am wondering what is the best practice. Another shop I know says they only use g92. But when running the test program if I don't set the relative and start points exactly the same then I can just be cutting air as I have since learned.

    I have used g54 mostly on the mills it makes a bit more sense to me. If I set a x0 y0 as the corner of my part for example and set that as G54 with the machine move to the correct starting point based on the G54 value.

    So if G54 is X0 Y0, and the start of the cut is at x1 y-1 will the machine move there first before starting the cut? If so what should my starting blocks look like?

    Thanks

  2. #2
    Join Date
    Aug 2006
    Location
    greensboro,northcarolina
    Posts
    2,335
    Post Thanks / Like
    Likes (Given)
    136
    Likes (Received)
    546

    Default

    Using G54 or G92 is really just a personal preference, either works . I would suggest understanding both clearly, then make the decision. Kind of depends on how you set things up and what kind of work you are doing.

  3. #3
    Join Date
    Jun 2016
    Country
    CANADA
    State/Province
    Ontario
    Posts
    38
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Do you have a code example of the differences between two.

  4. #4
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    79
    Post Thanks / Like
    Likes (Given)
    30
    Likes (Received)
    21

    Default

    I use G92 to assign machine position for the program being run. G54, G55 , G56 I use for each piece on the table.

    %
    L1/100
    (INCH)
    H001=000.00810
    (H900 RESERVED)
    H900=000.00000
    G70
    G90
    G92 X0.0 Y0.0
    Z1=0.000
    Z2=0.585
    Z5=1.170
    G00 X1.0 Y-1.0

  5. #5
    Join Date
    Jun 2016
    Country
    CANADA
    State/Province
    Ontario
    Posts
    38
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    How would that look if you used g54 instead of g92, just substitute it?

  6. #6
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,717
    Post Thanks / Like
    Likes (Given)
    305
    Likes (Received)
    1815

    Default

    Quote Originally Posted by tzak View Post
    How would that look if you used g54 instead of g92, just substitute it?
    Not a Mits user, but no, it won't.

    With G54 ( with no G92 actually ), you set the X and Y work coordinates when you pickup the edges ( or whatever you use to define the location )
    and then in your program you just move to wherever you want to start from and not have any G92 blocks.

    Basically, you can use it just like on the mills.

    For your example, let's say you pick up the L/R corner as X0 Y0, and set it for the G54 work coord.
    Then your program would look like:

    %
    L1/100
    (INCH)
    H001=000.00810
    (H900 RESERVED)
    H900=000.00000
    G70
    G90
    G54
    Z1=0.000
    Z2=0.585
    Z5=1.170
    G00 X1.0 Y-1.0
    G01 G42 X0 Y-1.0
    G01 X0 Y1.0
    G01 X-1.0 Y1.0
    G01 X-1.0 Y0
    G01 X1.0 Y0
    G01 G40 X1.0 Y-1.0
    M30

    That should cut a 1 x 1 square.

  7. #7
    Join Date
    Sep 2012
    Location
    California, Ventura county
    Posts
    1,403
    Post Thanks / Like
    Likes (Given)
    256
    Likes (Received)
    602

    Default

    that's kind of the same run around I got from bobcad
    for a Fadal post processor, long on promises short on delivery

  8. #8
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    40
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    11

    Default

    Quote Originally Posted by tzak View Post
    I purchased Bobcam wire and it has gone from them telling me they can modify a post processor in a couple weeks, into they can look at it 6-8 week after a month has passed (not pleased). Anyway now I have to modify and change the post on my own. It's not terribly difficult and if anyone has one for a Mitsubishi FX20 that would be great. But one thing I'm trying to understand is what benefits or differences are there to use G92 or G54 in programming for part setup to adjust the post accordingly.

    I had a test program with G92 and am wondering what is the best practice. Another shop I know says they only use g92. But when running the test program if I don't set the relative and start points exactly the same then I can just be cutting air as I have since learned.

    I have used g54 mostly on the mills it makes a bit more sense to me. If I set a x0 y0 as the corner of my part for example and set that as G54 with the machine move to the correct starting point based on the G54 value.

    So if G54 is X0 Y0, and the start of the cut is at x1 y-1 will the machine move there first before starting the cut? If so what should my starting blocks look like?

    Thanks
    I run a different type of machine but,if you set a "0" corner in G54 or any other work coordinate and give yourself a thread point then start to cut your machine will do just that. The only time I tend to use G92 is for sub programs when I am using multiple work coordinates.

    Example Program for a Diameter.
    I thread in the center so it rapids to x0 y0 then threads.

    N100 G90 ;
    N110 G54;
    N120 G00 X0. Y0. ;
    N130 T91 ;
    N140 C001 H001 ;
    N150 G01 G41 X.0939 Y-.0937 ;
    N160 G03 X.1876 Y0. I0. J.0937 ;
    N170 X-.1876 I-.1876 J0. ;
    N180 X.1876 I.1876 J0. ;
    N190 G50 X.0939 Y.0937 I-.0937 J0. ;
    N200 G01 G40 X0. Y0. ;
    N210 C002 H002 ;
    N220 G01 G42 X.0939 Y.0937 ;
    N230 G02 X.1876 Y0. I0. J-.0937 ;
    N240 X-.1876 I-.1876 J0. ;
    N250 X.1876 I.1876 J0. ;
    N260 G50 X.0939 Y-.0937 I-.0937 J0. ;
    N270 G01 G40 X0. Y0. ;
    N280 C003 H003 ;
    N290 G01 G41 X.0939 Y-.0937 ;
    N300 G03 X.1876 Y0. I0. J.0937 ;
    N310 X-.1876 I-.1876 J0. ;
    N320 X.1876 I.1876 J0. ;
    N330 G50 X.0939 Y.0937 I-.0937 J0. ;
    N340 G01 G40 X0. Y0. ;
    N350 C004 H004 ;
    N360 G01 G42 X.0939 Y.0937 ;
    N370 G02 X.1876 Y0. I0. J-.0937 ;
    N380 X-.1876 I-.1876 J0. ;
    N390 X.1876 I.1876 J0. ;
    N400 G50 X.0939 Y-.0937 I-.0937 J0. ;
    N410 G01 G40 X0. Y0. ;
    N420 T90 ;
    N430 M02 ;

  9. #9
    Join Date
    Jun 2016
    Country
    CANADA
    State/Province
    Ontario
    Posts
    38
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I wanted to bring this topic back us as I have done some more testing on the machine with regards to setting G54.

    I seem to have the post working with the main part of my program looking like so, no sub program.


    L100 / TEST G54
    (MACHINE MITSUBISHI FX-20 )
    G90
    G53 G92 X0. Y0.
    M20
    M78 M78 (Fill Tank)

    (2 AXIS ROUGH CUT)
    M102
    Z1=0.0000
    Z2=0.3543
    Z5=-0.7087
    G00 G90 G54 X-1.2205 Y.15 M91
    M80 (Fluid ON)
    M82 (Wire ON)
    M84 (Machining ON)
    E1421 F.160
    M90
    G01 G41 X-1.2205 Y0. H1=.0081
    X-1.2205 Y0.
    X-.0197 Y0.


    When I move the machine to my part setup I ZERO out my relative position and also make that my G54, (for this example). I can then move the machine anywhere on the table start the job up and the machine will position back to the G54. And the G54 and relative numbers are exactly the same. So the code is doing what it is supposed from what I can understand.

    Here is the problem.

    I have been setting up my job with a coordinate rotation. Meaning the part is not square in the machine. The machine can calculate this angle and then reset the X an Y to match the new angle making it square for cutting.

    When calling up the G53 command at the start of the program with this rotation, the machine thinks the rotation angle is from the machine calibration point (machine 0,0 g53) and is compensating for the angle difference from that point. The further I move away from g53 the larger this number gets between the relative number I what I set ford my G54. If I turn off the rotation then both readouts are correct and the same. If I leave rotation ON the machine does no go to the place I set G54. Now in running jobs I usually use this rotation because I don’t square up parts to the table very often. How can I have the system ignore the rotation based on the g53 from X0 yY0? Having to square up all material is not a realistic option all the time but I'm sure that this can be solved with some G code tweak. Or a way to zero out the g54 to match where the actual X0 Y0 in my program is.

    Hope someone can clarify this issue for me.

    thanks

  10. #10
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    79
    Post Thanks / Like
    Likes (Given)
    30
    Likes (Received)
    21

    Default

    Quote Originally Posted by tzak View Post
    I wanted to bring this topic back us as I have done some more testing on the machine with regards to setting G54.

    I seem to have the post working with the main part of my program looking like so, no sub program.


    L100 / TEST G54
    (MACHINE MITSUBISHI FX-20 )
    G90
    G53 G92 X0. Y0.
    M20
    M78 M78 (Fill Tank)

    (2 AXIS ROUGH CUT)
    M102
    Z1=0.0000
    Z2=0.3543
    Z5=-0.7087
    G00 G90 G54 X-1.2205 Y.15 M91
    M80 (Fluid ON)
    M82 (Wire ON)
    M84 (Machining ON)
    E1421 F.160
    M90
    G01 G41 X-1.2205 Y0. H1=.0081
    X-1.2205 Y0.
    X-.0197 Y0.


    When I move the machine to my part setup I ZERO out my relative position and also make that my G54, (for this example). I can then move the machine anywhere on the table start the job up and the machine will position back to the G54. And the G54 and relative numbers are exactly the same. So the code is doing what it is supposed from what I can understand.

    Here is the problem.

    I have been setting up my job with a coordinate rotation. Meaning the part is not square in the machine. The machine can calculate this angle and then reset the X an Y to match the new angle making it square for cutting.

    When calling up the G53 command at the start of the program with this rotation, the machine thinks the rotation angle is from the machine calibration point (machine 0,0 g53) and is compensating for the angle difference from that point. The further I move away from g53 the larger this number gets between the relative number I what I set ford my G54. If I turn off the rotation then both readouts are correct and the same. If I leave rotation ON the machine does no go to the place I set G54. Now in running jobs I usually use this rotation because I don’t square up parts to the table very often. How can I have the system ignore the rotation based on the g53 from X0 yY0? Having to square up all material is not a realistic option all the time but I'm sure that this can be solved with some G code tweak. Or a way to zero out the g54 to match where the actual X0 Y0 in my program is.

    Hope someone can clarify this issue for me.

    thanks
    I use rotation all the time, different angles with multiple different pieces on the machine table all at the same time.

    You need to have Coordinate rotation off it does not like to work with workpoints from my experience ... Workpoints like G54 G55 G56 are for multiple pieces. So do this during your setup: get the angle using coordinate or rotation but plug that angle in the program as "K" rotation.

    %
    K23.512
    L1/101
    (INCH)
    H001=000.00520
    (H900 RESERVED)
    H900=000.00000
    G70
    G90
    G92 X0.0 Y0.0
    Z1=0.125
    Z2=0.0625
    Z5=0.0
    G00 X0.0 Y-0.3
    M20
    M78 M78
    M80
    M82
    E951 F0.075 H1
    M84
    G01 G42 X0.0 Y-0.08125 M90
    E3652 F0.05
    G03 X0.04747 Y0.06594 I0.0 J0.08125
    G02 X0.05039 Y0.075 I0.00292 J0.00406
    G01 X0.10139 Y0.075
    X-0.12021 Y0.075
    X-0.12021 Y0.085
    X-0.10139 Y0.085
    X-0.10139 Y0.075
    X-0.05039 Y0.075
    G02 X-0.04747 Y0.06594 I0.0 J-0.005
    G03 X-0.03393 Y-0.07383 I0.04747 J-0.06594
    M01
    M80
    M82
    M84
    X0.0 Y-0.08125 I0.03393 J0.07383
    G01 G40 X0.0 Y-0.11125
    M91
    M21
    G00 X0.0 Y0.0
    K0.0
    G23
    %

    Hope this helps.


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
  •