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

Page 1 of 2 12 LastLast
Results 1 to 20 of 28
  1. #1
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    6,447
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1733

    Default G43 and more than one axis in line

    i use a CNC gantry mill with vertical and horizontal head so when G43 used normally it is
    G0 G43 H1 Z20.
    .
    instead of
    G0 G43 H1 X0. Y0. Z20.
    ..... as if multiple axis in line the length comp will effect every axis in line. on a cnc where it can point to +X or -X, +Y or -Y or -Z the cnc does not know which axis G43 should effect. but on 3 horizontal cnc's i use nearby if more than one axis in line G43 only effects Z
    .
    is it more normal in gcode if more than one axis in gcode line where G43 used length comp only effects Z ?? can others have
    G0 G43 H1 X0. Y0. Z20. and length comp only effects Z ??
    maybe it is a parameter setting ? i was told it is safer to use
    G0 X0. Y0.
    G0 G43 H1 Z20.
    or only one axis in line where G43 used. i am just wondering maybe only important on 5 axis machine or only a few CNC

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

    Default

    Can't speak of the rest since I've only used a Haas control, but how would G43 affect X or Y when it is length offset? Should only be Z... one would think.

    Normal 3axis stuff I do XY first, then G43Z. But sometimes on 4axis stuff, I have a post which outputs G43H XYZA and have no issues. Eg: G0 G90 G59 X0.4585 Y-3.433 G43 H13 Z4. A90. /M8

  3. #3
    Join Date
    Jan 2014
    Location
    Vancouver, WA. USA
    Posts
    1,984
    Post Thanks / Like
    Likes (Given)
    435
    Likes (Received)
    892

    Default

    There are parameters that affect how G43 is applied on many CNCs. What control are you referring to?

  4. #4
    Join Date
    Oct 2005
    Location
    Wilmington DE USA
    Posts
    1,576
    Post Thanks / Like
    Likes (Given)
    227
    Likes (Received)
    285

    Default

    gantry with horizontal head I'm guessing you need to define the "Y" offset

  5. #5
    Join Date
    Aug 2013
    Location
    Duluth, Mn
    Posts
    343
    Post Thanks / Like
    Likes (Given)
    46
    Likes (Received)
    101

    Default

    My question to you is. What is the reason for this? Are you trying to save a small amount of cycle? Is some programmer adding it for the hell of it?

    G00 X Y
    G43 H Z

    is used to control the machine movement as expected

    G43 H X Y Z

    I could see resulting in a compound move.

  6. #6
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    6,447
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1733

    Default

    Quote Originally Posted by Vancbiker View Post
    There are parameters that affect how G43 is applied on many CNCs. What control are you referring to?
    .
    .
    Fanuc 15 both machine types the gantry mill with vert and horz attachments and the just horizontal mills
    .
    gantry mill with horz attachment you can be using G18 or G19 (instead of G17) and G43 or G44 depending on which way it is pointing to + or -. presently comp effects all axises in line when G43 used and control has no way of knowing which axis to select so all axis in gcode line affected
    .
    when milling this would effect X and Y and Z if all in G43 line and has caused scrap before. when i saw in horizontal cnc gcode
    G0 G43 H1 X0. Y0. Z20. i thought it was a mistake and changed to
    G0 X0. Y0.
    G0 G43 H1 Z20.
    ..... but when i tried it in mdi i saw only Z effected when all 3 axis in G43 line. thats why i assumed it is a parameter thing. some parameter must be G43 only effects Z
    .
    i was at a job interview once and it came up in discussion with interviewer never hearing of G43 effecting any other axis. so he thought i was inexperienced and did not know what i was talking about. it was more my experience was with different cnc machines which act different. i had assumed all cnc act the same and job interviewer thought like wise but we each had experience with different cnc's which act different

  7. #7
    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 deljr15 View Post
    My question to you is. What is the reason for this? Are you trying to save a small amount of cycle? Is some programmer adding it for the hell of it?

    G00 X Y
    G43 H Z

    is used to control the machine movement as expected

    G43 H X Y Z

    I could see resulting in a compound move.
    That's exactly the case for me. It does save time, especially on very long parts when you have to do things at opposite ends and have a large Z travel, combined with many tool changes, like on our VF7.

    Also helps save time with a slow rotary like the HRT models. Move the rotary axis at same time as XY, or on most of the parts I do I just use XYZA. Normally to a safe Z-plane above part, then down to first rapid height of the toolpath.

  8. #8
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    98
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    45

    Default

    I am confused to why you would have X0 Y0 in the same line as the G43.

  9. #9
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    6,447
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1733

    Default

    Quote Originally Posted by deljr15 View Post
    My question to you is. What is the reason for this? Are you trying to save a small amount of cycle? Is some programmer adding it for the hell of it?

    G00 X Y
    G43 H Z

    is used to control the machine movement as expected

    G43 H X Y Z

    I could see resulting in a compound move.
    .
    .
    i am just operator and i saw
    G43 H1 Z20.
    and a few lines lower i see
    G0 G43 H1 X0. Y0. Z20.
    .
    i am thinking it is just the Cad Cam program how it is setup. probably can be changed in Cad Cam program. often post processor is not perfect and programmer corrects post processor mistakes. i thought at first it was just something programmer missed. he has missed a few over the years. little things like G17 called a few lines after G19 and G17 was a post processor default setting has caused problems before in that G17 should never have been called with horizontal head pointing in X or Y direction

  10. #10
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    6,447
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1733

    Default

    Quote Originally Posted by thesidetalker View Post
    That's exactly the case for me. It does save time, especially on very long parts when you have to do things at opposite ends and have a large Z travel, combined with many tool changes, like on our VF7.

    Also helps save time with a slow rotary like the HRT models. Move the rotary axis at same time as XY, or on most of the parts I do I just use XYZA. Normally to a safe Z-plane above part, then down to first rapid height of the toolpath.
    .
    i got no problems with
    G0 G43 H1 Z30.
    G0 X0. Y0. Z20.
    or 3 axis move after length comp called not in middle of length comp line

  11. #11
    Join Date
    Jan 2014
    Location
    Vancouver, WA. USA
    Posts
    1,984
    Post Thanks / Like
    Likes (Given)
    435
    Likes (Received)
    892

    Default

    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.

  12. #12
    Join Date
    Jul 2012
    Location
    Washington
    Posts
    1,657
    Post Thanks / Like
    Likes (Given)
    517
    Likes (Received)
    606

    Default

    Quote Originally Posted by Shawnrs View Post
    I am confused to why you would have X0 Y0 in the same line as the G43.
    Are you an employee or is it your gig? Doing as much on each line of code saves time, quite a lot if you do production. On my drill/tap machines it probably saves a second per tool change. I do a lot of tool changes every year. This has never been the cause of any crash for me, but they are worse when running the spindle into the part rapiding in both X and Z, especially linear way machines.

  13. #13
    Join Date
    Jan 2007
    Location
    Flushing/Flint, Michigan
    Posts
    5,510
    Post Thanks / Like
    Likes (Given)
    207
    Likes (Received)
    4341

    Default

    So I know you change which axis the length comp goes to in the parameters.
    But will it trigger off of the axis specified in a line.
    Is G43 H1 with no axis a legal line? Perhaps surprising results if you have 10 inches in H1 or an overtravel but legal if say H1 was .001?
    Bob

  14. #14
    Join Date
    Jan 2003
    Location
    Tel Aviv, Israel
    Posts
    460
    Post Thanks / Like
    Likes (Given)
    51
    Likes (Received)
    76

    Default

    I used the G43H**X**/Y**/Z** expressions for FANUC probe measuring programs while using Star type stylus, or measuring tool length in 90deg milling attachment.

    In all my cases it worked correctly, with following syntax:

    G17
    G43H**Z***

    or

    G18
    G43H**Y***

    or

    G19
    G43H**X***

  15. Likes Rstewart, thesidetalker liked this post
  16. #15
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    98
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    45

    Default

    Quote Originally Posted by DavidScott View Post
    Are you an employee or is it your gig? Doing as much on each line of code saves time, quite a lot if you do production. On my drill/tap machines it probably saves a second per tool change. I do a lot of tool changes every year. This has never been the cause of any crash for me, but they are worse when running the spindle into the part rapiding in both X and Z, especially linear way machines.
    In all the years of programming I have never seen it used in the same line with the G43. Every program I make or have seen usually looks something like this G43 H01 Z.15 M8. If I am drilling the G99/G98 take an effect and in most cases I use the G98 which uses the G43 line as the retract. If I am programming a job that has a fixture or clamps in the way I set the G43 Z to clear the clamps or fixture and use a G99.

  17. #16
    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 PROBE View Post
    I used the G43H**X**/Y**/Z** expressions for FANUC probe measuring programs while using Star type stylus, or measuring tool length in 90deg milling attachment.

    In all my cases it worked correctly, with following syntax:

    G17
    G43H**Z***

    or

    G18
    G43H**Y***

    or

    G19
    G43H**X***
    Damn, that's pretty neat. Didn't know G43 could be used like that in the other arc planes. Makes sense!

  18. #17
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    6,447
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1733

    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.
    .
    .
    i will see if my machine uses same parameter.
    .
    i have seen when more than one axis in G43 line and comp affected every axis caused the scrap of $5000. castings.
    .
    the time savings maybe in 1000 years would pay for higher speed but i am not interested in saving seconds and scrapping big parts. i myself would rather be cautious and have easier to read gcode of
    G43 H1 Z10.
    .
    on a gantry mill the quill extension is Z but the main columns are W it is also possible to use G43 H1 W10.
    .
    so apparently many cnc allow more than one axis in G43 line and tool length comp only effects Z cause a parameter can be set so it ignores comp change on any other axis. this would explain why some never heard of any problems with multiple axis in G43 line

  19. #18
    Join Date
    Jul 2012
    Location
    Washington
    Posts
    1,657
    Post Thanks / Like
    Likes (Given)
    517
    Likes (Received)
    606

    Default

    Quote Originally Posted by thesidetalker View Post
    Damn, that's pretty neat. Didn't know G43 could be used like that in the other arc planes. Makes sense!
    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.

  20. #19
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    6,447
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1733

    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.
    .
    .
    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
    Attached Thumbnails Attached Thumbnails bn-25a_horz_2014july28c.jpg  

  21. #20
    Join Date
    Jul 2012
    Location
    Washington
    Posts
    1,657
    Post Thanks / Like
    Likes (Given)
    517
    Likes (Received)
    606

    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
    Not on my Yasnac J50 control. G43/44 only works in the Z axis.


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
  •