Setting Offsets (G54) in ShopTurn with 810D
Close
Login to Your Account
Results 1 to 7 of 7
  1. #1
    Join Date
    Jul 2018
    Country
    UNITED KINGDOM
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    1

    Default Setting Offsets (G54) in ShopTurn with 810D

    Edit: I meant to write "Siemens 810D Control" in title. Doesn't look like it's possible to edit titles.


    Hi All

    New to post here but been here for a while.

    For a while now I've been trying to workout if there is a GCode line I can use to set the work offset with ShopTurn on a Siemens 810D control (the machine is a Hardinge).

    I've googled it and read some manuals but could never get it to work. I want to just add a line at the top of the program to set the G54 for each program.

    For example I'd like to set the Z G54 work offset to 100mm.
    In normal gcode that would be something like "G10 L2 P1 G90 Z100.0" I can't get this to work with this control though. Does any one have experience with ShopTurn/Siemens controls?

    I'm sure it must be something simple.

    Thanks in advance
    Last edited by mattdlr; 02-09-2021 at 10:49 AM. Reason: Clarify title

  2. Likes Ox liked this post
  3. #2
    Join Date
    Mar 2008
    Location
    vacaville ca
    Posts
    549
    Post Thanks / Like
    Likes (Given)
    85
    Likes (Received)
    150

    Default

    you can do a

    trans z100

    its part of the frames concept of seimens. trans by itself will cancel the frame completely. so if you had x or y transformations it cancels them to

  4. #3
    Join Date
    Feb 2004
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3,943
    Post Thanks / Like
    Likes (Given)
    1196
    Likes (Received)
    1955

    Default

    My 810D is on an Emco Maier, we use

    G58 X0 Z100 (Shift Z100mm)
    G58 X0 Z0 (Cancel Z shift)

  5. #4
    Join Date
    Jul 2018
    Country
    UNITED KINGDOM
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    1

    Default

    Thanks for the responses. TRANS puts an offset into the program only which will probably work. I was hoping to be able to set my work offset (G54) from the program and it stay set even after the program ends.

    SIM, G58 doesn't do anything, is G58 the work offset that you use or do you use G58 as a means to set a work offset? Either way my machine errored out when I tried "G58 X0 Z100."

    Off topic but do either of you use a network/computer attached to your Siemens 810D (I've never managed to get it to work)?

  6. #5
    Join Date
    Mar 2008
    Location
    vacaville ca
    Posts
    549
    Post Thanks / Like
    Likes (Given)
    85
    Likes (Received)
    150

    Default

    try this


    $P_UIFR[1]=CTRANS(Z,11.500) ; G54
    $P_UIFR[2]=CTRANS(Z,43.710) ; G55
    $P_UIFR[3]=CTRANS(Z,22.222) ; G56
    $P_UIFR[4]=CTRANS(Z,22.222) ; G57

  7. Likes mattdlr, Ox liked this post
  8. #6
    Join Date
    Jul 2018
    Country
    UNITED KINGDOM
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    1

    Default

    Thank you, that's exactly what I was after!

  9. #7
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    27,217
    Post Thanks / Like
    Likes (Given)
    7646
    Likes (Received)
    9457

    Default

    I use G10 to load the Fanuc's like that, but I never knew the Siemens way.

    I may implement that as well.
    Thanks!


    -----------------------

    Think Snow Eh!
    Ox


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
  •