G43 and more than one axis in line - Page 2
Largest Manufacturing Technology
Community On The Web
Close
Login to Your Account

Page 2 of 2 FirstFirst 12
Results 21 to 28 of 28
  1. #21
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    348
    Post Thanks / Like
    Likes (Given)
    55
    Likes (Received)
    170

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    .
    G43 AND G44 is used on any axis. G43 or G44 depends on if pointing at -X or +X same with Y. about only direction fixed is Z pointing toward -Z
    If you always use negative tool lengths, sure. With a probe or tool setter using positive lengths, that's not the case. The spindle offset is positive. Put a G49 on a line by itself and watch your spindle squash the tool into part/vise/table when it moves down.

  2. #22
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    348
    Post Thanks / Like
    Likes (Given)
    55
    Likes (Received)
    170

    Default

    Quote Originally Posted by DavidScott View Post
    This does not always work, depends on the control, and parameters as I am finding out. It can be handy if your control doesn't have fixture offsets, like a Fanuc 3.
    Does that work on Haas?

  3. #23
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    6,443
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1732

    Default

    Quote Originally Posted by thesidetalker View Post
    If you always use negative tool lengths, sure. With a probe or tool setter using positive lengths, that's not the case. The spindle offset is positive. Put a G49 on a line by itself and watch your spindle squash the tool into part/vise/table when it moves down.
    .
    always more - comp will cut deeper and more + will cut less on most machines
    .
    i have used a Mazak mill that was backwards or more + on length comp cut more. yet mazak lathe next to it was normal more - cuts more......... most likely a parameter setting
    .
    G43 and G44 if tool is -.500 length comp the G43 or G44 will control which direction comp goes depends on which direction spindle pointing. i always remember
    if spindle points to negative direction use G43
    if spindle points to positive direction use G44
    .
    since in Z normally spindle only points toward negative only G43 is just normally used with Z axis
    .
    but with a parameter setting change probably anything is possible and any machine can act differently

  4. #24
    Join Date
    May 2006
    Location
    Burlington, North Carolina
    Posts
    134
    Post Thanks / Like
    Likes (Given)
    111
    Likes (Received)
    55

    Default

    Our Daewoo with a Fanuc 21i will work either way. I just always got in the habit of doing

    G0 X Y

    G43 H Z0.1

    In case there were clamps in the way and what-not.

  5. #25
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    6,443
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1732

    Default

    Quote Originally Posted by Vancbiker View Post
    Check out parameter 6000 bit 4 in your manual. I think you will see this is where the ability to have the G43 only affect Z or affect any named axis is determined.
    .
    .
    yes that screen says cutter comp and line has 0 and 1's like
    00010001
    .
    no way i would change it as machine runs ok for decades. but nice to know it can be changed. now if talking about it to other machinist and they disagree on only 1 axis in G43 line than i can mentioned it can be changed by parameters

  6. #26
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    6,443
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1732

    Default

    Quote Originally Posted by thesidetalker View Post
    If you always use negative tool lengths, sure. With a probe or tool setter using positive lengths, that's not the case. The spindle offset is positive. Put a G49 on a line by itself and watch your spindle squash the tool into part/vise/table when it moves down.
    .
    .
    my machines use wear comp
    .
    if a tool has max length of 10" gage length and comp of -.500 cause it is 9.5000 GL the programming uses the 10" length. if G49 or no length comp in effect it stays farther away as tool is always shorter than max length used for programming
    .
    wear comp only, often is used in normal comp columns on cnc
    .
    main reason is it prevents crashes of no G43 is in effect or rather tool is farther away. i have seen a (tap) drill, drill hole shallow, then next tool a tap hit bottom of hole. thats a rare case where wear comp still can cause a problem

  7. #27
    Join Date
    Jan 2014
    Location
    Vancouver, WA. USA
    Posts
    1,983
    Post Thanks / Like
    Likes (Given)
    434
    Likes (Received)
    891

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    .
    yes that screen says cutter comp and line has 0 and 1's like
    00010001
    .
    no way i would change it as machine runs ok for decades. but nice to know it can be changed. now if talking about it to other machinist and they disagree on only 1 axis in G43 line than i can mentioned it can be changed by parameters
    Changing 00010001 to 00000001 will make G43 effective only in Z regardless of other axes called on the G43 line.

    For a non head changing machine that is the usual setting. If you have a head changer or use angle heads then you want it set as it is.

  8. #28
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    6,443
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1732

    Default

    Quote Originally Posted by Vancbiker View Post
    Changing 00010001 to 00000001 will make G43 effective only in Z regardless of other axes called on the G43 line.

    For a non head changing machine that is the usual setting. If you have a head changer or use angle heads then you want it set as it is.
    .
    .
    interesting, nice that it can be changed but i will leave the 4 cnc i use as is.
    .
    the 3 horizontal cnc are set with more precautions to prevent crashes from inexperienced operators or just mistakes. the gantry cnc mill requires being extra careful. restarts require checking for G92 shift and seeing what G and M codes in effect. the horizontals are setup with (RESTART HERE) often in programs. saves a lot of scrap parts from happening


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
  •