Results 1 to 10 of 10

Thread: Mach 3 work offset retention.

  1. #1
    Registered
    Join Date
    Oct 2006
    Location
    United Kingdom
    Posts
    8
    Downloads
    0
    Uploads
    0

    Post Mach 3 work offset retention.

    I am new to using Mach 3 and on a "learning curve " It's all working OK on a mill but when I put in the work offset no 1 (G54) and save it - it has not been retained at start up the next day. I have read the manual and set the box on the config screen to persistent offsets.
    I must be missing something.

    Similar Threads:


  2. #2
    Registered
    Join Date
    Aug 2006
    Location
    usa
    Posts
    65
    Downloads
    0
    Uploads
    0

    Default

    I have Mach 3 and I reset my G54 offsets every day. When I shut the machine down the next day it's blank when I start up. I used the machine yesterday and as I read your post I went and checked it out and it was clean nothing retained. To many variables to say that your X0Y0Z0 will be in the same place when you shut down and start up again, and if you have stepper motors you have to zero every time as sometimes they want to creep. I only cut wood and I always leave plenty of stock.Maybe it's a good thing it does not retain the G54 you may get lazy and not check and scrap your next part. I downloaded all 154 pages of Mach3 I will read thru and see if there is anything on the subject. Art has a great product going with the the Mach 3, and has great service.

    9lrac9 K2cnc owner.



  3. #3
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Twp, MI....USA
    Posts
    24644
    Downloads
    0
    Uploads
    0

    Default

    G54 Is the default coordinate system, so it doesn't get saved. There's a workaround, however. On the offset screen, click "Save Offsets". Scroll down to the last one, G59P253. Set up your offsets there and save.

    Open the General Configuration screen. At the bottom right side, check the box that says "copy G54 from G59.253 at startup". Restart Mach3 and you'll have your G54 offsets.

    Gerry

    Mach3 2010 Screenset
    http://home.comcast.net/~cncwoodworker/2010.html

    JointCAM
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  4. #4
    Registered
    Join Date
    Dec 2003
    Location
    keski- suomi, FINLAND
    Posts
    18
    Downloads
    0
    Uploads
    0

    Default

    To have G54 saved you need these settings made:
    From general config,
    Axis DRO properties:

    Optional Offset Save
    Persistent DROs

    Above must be selected, all others must NOT be selected, most important unselected is "Copy G54 from G59.253 on startup" if it is selected Mach will allways when started copy work offsets from G59P253.

    -Mika



  5. #5
    Registered
    Join Date
    Oct 2006
    Location
    United Kingdom
    Posts
    8
    Downloads
    0
    Uploads
    0

    Smile Work Offset retention - thanks

    Gerry / Mika - Many thanks for your comments. I appreciate your help.
    I tried the configuration as per your suggestion today and it works perfectly ! Thanks again.

    Geoff



  6. #6
    Registered
    Join Date
    Apr 2007
    Location
    Lithuania
    Posts
    14
    Downloads
    0
    Uploads
    0

    Default

    Hello,

    Although this post is old, but still fits my question, so...

    This thing with G53, G54 and so on still confuses me. Today i had some problems with milling using G code, generated with solidcam (found postpocessor on this forum). Solidcam added all those codes in the beginning and end of program. I needed to cut out few identical parts. The first one went fine. After that i moved tool back to X0Y0Z20 and then moved to X242Y0Z20, where second part should be cut and then zeroed the X coordinate, regenerated toolpath. But when i started the program, it went to wrong coordinates. Here is the program code:

    %
    O1 (FREZAVIMUI)
    N5 G0 G40 G49 G80 G21 (Initialisation)
    N10 G0 G53 Z0 (Retour aux origines machine)
    N15 G0 G53 X0 Y0
    N20 (Outil n 1 - Diametre 6.3 D1 H1)
    N25 T1 M6 D1 H1
    N30 S1000 M4
    N35 M8
    N40 (P-contour7-T1)
    N45 G0 G55 X-4.33 Y3.44
    N50 G43 H1 Z10.
    N55 G0 Z2. (this is where the tool positions to enter the material and milling begins)
    N60 G1 X4.33 Y8.44 Z-2. F300

    <...>

    N1735 G0 Z10.
    N1740 G0 G53 Z0 M9
    N1745 G0 G53 X0 Y0 M5
    M30
    %
    N10, N15, N45, N50, N1740 and N1745 lines are the ones, which i can't fully understand. What does mach3 do when it runs these lines and how can i replace them with a simple starting position? Also i manually change tools and spindle speed, so i suppose i can simply delete N25, N30, N35 lines.



  7. #7
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Twp, MI....USA
    Posts
    24644
    Downloads
    0
    Uploads
    0

    Default

    N10 and N1740 move the machine to machine coordinate Z0.

    N15 and N1745 move the machine to machine coordinate X0Y0.

    You can probably remove these lines if you don't need them.

    Default coordinate system in Mach3 is G54. Your part is using G55. When you re zero for your second part, you need to make sure you're in G55 when you do that. It's possible your setting the zero in G54.

    You can use any coordinate system (offset) you want. G54,G55,G66... Each may have a different 0,0,0 origin position. You need to make sure you set your zero position in the same offset your program is using.

    Gerry

    Mach3 2010 Screenset
    http://home.comcast.net/~cncwoodworker/2010.html

    JointCAM
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  8. #8
    Registered
    Join Date
    Apr 2007
    Location
    Lithuania
    Posts
    14
    Downloads
    0
    Uploads
    0

    Default

    I am totaly knew to this offseting stuff, so don't bite if i sound stupid . Its just that i'm having problems understanding stuff if no samples are provided, not to mention, that its not easy to understand in english, since its not my mother-tongue.

    So correct me if i am wrong: basicaly, G54-G59 are simply temporary coordinate systems inside main coordinate system?

    I have found a picture in one book:



    And here's how it was explained :
    By means of G52 the local coordinate system (X'Y'Z') will be assigned, which onset will be offset
    relative to operative XYZ so, that tool current point in coordinate local system will accept a value of
    the amounts specified in addresses X,Y,Z.
    For example, while assignment G52X100Y100, coordinate local system will set relative to operative
    offset on vector A (100,60) (see pic. 11) and tool current point will become equal to X100, Y100
    instead of X200, Y160.
    So XYZ coordinates are set using G53 or G54-59? And shouldn't X'Y'Z' coordinates be set using G52X100Y60 (not Y100) in this case?

    If i understand correct, then G53 command sets my machine coordinate system, which tells me, where my tool is actually on my machine, then G52 sets temporary new coordinate system in program, which will be used as boundaries to work inside (for eg. corner of my stock material). And finally, using G54-G59 i can set temporary coordinate systems inside those boundaries (for eg. several identical parts needed to cut on that stock) right?



  9. #9
    Community Moderator ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Twp, MI....USA
    Posts
    24644
    Downloads
    0
    Uploads
    0

    Default

    G53 is the machine coordinates. When you home your machine, it zero's the machine coordinates.

    G54 is the default coordinate system in Mach3. After you home the machine, you will be in the G54 coordinate system, and any offsets will be applied in reference to the machine coordinates. If your G54 offsets are all zero, then G54 will be the same as G53.

    G54,G55,G56, ... are all independent coordinate systems, with their offsets relative to the G53 machine coordinates.

    If you want to have different 0,0 position on your machine, possibly for different fixtures, you can set a specific offset to reference that fixture, and just call that offset before running the part.

    I once ran a few parts and wanted them 3" apart along the X axis. I set the following offsets:

    G54 - X0
    G55 - X3
    G56 - X6
    G57 - X9

    Run one part, and switch to G55. Run next part, and switch to G56. Run next part, and switch to G57.

    G52 changes the offsets in the current coordinate system. If you use G52, you need to be careful to reset it so you know where you are.

    Gerry

    Mach3 2010 Screenset
    http://home.comcast.net/~cncwoodworker/2010.html

    JointCAM
    http://www.g-forcecnc.com/jointcam.html

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  10. #10
    Registered
    Join Date
    Apr 2007
    Location
    Lithuania
    Posts
    14
    Downloads
    0
    Uploads
    0

    Default

    Thanks, ger21. Now i think i understand. Gonna make some experimental moves on mach3 without a tool tomorrow.

    Just one more question from my previous post:

    And shouldn't X'Y'Z' coordinates be set using G52X100Y60 (not Y100) in this case?




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 from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed