G0G91G28Z0. cancelling G43 offset
Close
Login to Your Account
Results 1 to 19 of 19
  1. #1
    Join Date
    Jul 2021
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default G0G91G28Z0. cancelling G43 offset

    Hello,

    We have a Fanuc Oi-MF control on an Awea AV1000 mill.

    If G43 H4 is active for the tool length offset and I do a G0G91G28Z0 or if I do G0G91G30Z0 the H4 value is cancelled.

    If you look at the position check screen where you can see all active G-codes and H & T values it still shows the H4 as being active but it is definitely not active anymore after the machine returns to zero return or 2nd zero return.

    I am fairly certain this is a parameter issue. If someone can tell me the parameter to change it would be greatly appreciated.

    Thanks!

  2. #2
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    27,661
    Post Thanks / Like
    Likes (Given)
    8002
    Likes (Received)
    9743

    Default

    This app is only barely in my wheelhouse, but when you punch in G28, that runs off of "Machine Zero" or whatnot.
    It has to dump any tool, fixture, or G10 offsets to make this move.

    Now - you say that it is still showing active in your list, and if so - then it only disregarded it for the G28 move, but maybe it is still active should you want to continue for some reason from a G28 position - although that seems an odd application.

    What is it that you are expecting - or desire it to doo differently?


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

    Think Snow Eh!
    Ox

  3. #3
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    766
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    274

    Default

    Not sure why you're running home and then back again with the same tool, unless there's some in program clearance you're after. Your problem might be that I don't see a G90 mentioned after all your G91 activity. Perhaps your machine is returning to work under an Incremental mindset.

    Another route is use G53 instead of G28. Simpler way to obtain the same movements, and it won't take you out of Absolute Mode.

  4. #4
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,170
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1778

    Default

    Quote Originally Posted by 13engines View Post
    Another route is use G53 instead of G28. Simpler way to obtain the same movements, and it won't take you out of Absolute Mode.
    The Tool Length Offset is also cancelled by G53.

    @markgerke
    Check carefully that the Tool Length Offset is still active with the next Z Move in Absolute Mode, as it should be restored.

    Regards,

    Bill

  5. #5
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,833
    Post Thanks / Like
    Likes (Given)
    1202
    Likes (Received)
    1975

    Default

    Check to see if G49 is active. That's what cancels tool offset.
    The H value would be the last H value read.

    If you called G43 with no H, it would use the active H (in your case H4)

  6. #6
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,126
    Post Thanks / Like
    Likes (Given)
    936
    Likes (Received)
    537

    Default

    Another curve to G53...if you're just sending the Z home out the way, you could just turn your rotary knob to the "home/zero return" position and hit the Z home button.
    Less typing...

  7. #7
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,170
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1778

    Default

    Quote Originally Posted by Booze Daily View Post
    Check to see if G49 is active. That's what cancels tool offset.
    The H value would be the last H value read.

    If you called G43 with no H, it would use the active H (in your case H4)
    Hello BD,
    Not necessarily, it depends on the setting of parameter bit 5001.2. If set to "0", that's correct. If set to "1", then Offset H00 will be made active, which is the same as cancelling the Offset as H00 has the value Zero and can't be set otherwise.

    Regards,

    Bill

  8. #8
    Join Date
    Sep 2009
    Country
    NEW ZEALAND
    Posts
    128
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    46

    Default

    So, I've always wondered why Fanuc(and simaler) use separate diameter/length offsets.

    Is there a practical reason or is is some legacy thing from older controls.

    I'm sure there's a good reason I just can't think of one.
    (So I'm coming from Heidenhain where the tool call contains all the info and tool lengths aren't cancelled (well I suppose they are temporarily)
    by moving in machine coords etc)

  9. #9
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,126
    Post Thanks / Like
    Likes (Given)
    936
    Likes (Received)
    537

    Default

    (New) Siemens is the same as Heidi - you just call your tool and the control automatically assigns your H+D because why would you use another number.

    Well, if you're interpolating a couple of tight features with the same tool number...you can then control exactly what you want for each feature with a separate D#
    (obviously you can do it other ways but this is an option...)

  10. #10
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    27,661
    Post Thanks / Like
    Likes (Given)
    8002
    Likes (Received)
    9743

    Default

    Quote Originally Posted by srp61 View Post
    So, I've always wondered why Fanuc(and simaler) use separate diameter/length offsets.

    Is there a practical reason or is is some legacy thing from older controls.

    I'm sure there's a good reason I just can't think of one.
    (So I'm coming from Heidenhain where the tool call contains all the info and tool lengths aren't cancelled (well I suppose they are temporarily)
    by moving in machine coords etc)

    In case you want slightly different offsets for the same tool.

    ex:

    Maybe doo to tool pressure, you may want a slightly smaller D on a longer cut surface than on a shorter wall surface?


    Not sumpthing that comes up all that often, but .....



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

    Think Snow Eh!
    Ox

  11. Likes mhajicek liked this post
  12. #11
    Join Date
    Nov 2005
    Location
    Santa Barbara
    Posts
    316
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    101

    Default

    I sometimes use different D's when I have to turn big and small tight diameters with the same tool. If you need a 16" diameter on the back, and a 1/4" on the front, a slight offset in Y can easily cost you a few tenths. Separate D's let you tune them both in, without shimming up the tool.

    On mills, I have engineers who like giving one sided tolerances. Sometimes I'll miss it when I'm programming. At the machine, it's easier to add a new D, than to fingercam a bigger/smaller tool path for that one sloppy callout.

  13. #12
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    2,013
    Post Thanks / Like
    Likes (Given)
    2744
    Likes (Received)
    1407

    Default

    Quote Originally Posted by Ox View Post
    In case you want slightly different offsets for the same tool.
    Exactly. I've run several jobs lately in which a given tool will have two or three different D offsets for dialing in different features.

  14. #13
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,126
    Post Thanks / Like
    Likes (Given)
    936
    Likes (Received)
    537

    Default

    Another way to adjust the tool (keeping the same offset number) for tight features, that i've just come across and used this week, is by using the attached.
    Attached Thumbnails Attached Thumbnails capture.jpg  

  15. #14
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,701
    Post Thanks / Like
    Likes (Given)
    1009
    Likes (Received)
    3220

    Default

    Quote Originally Posted by barbter View Post
    Another way to adjust the tool (keeping the same offset number) for tight features, that i've just come across and used this week, is by using the attached.
    That method can be ok, but without some care in programming can result in trouble should the program be aborted mid operation. Using alternate D addresses has fewer pitfalls.

  16. #15
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,126
    Post Thanks / Like
    Likes (Given)
    936
    Likes (Received)
    537

    Default

    Quote Originally Posted by Vancbiker View Post
    That method can be ok, but without some care in programming can result in trouble should the program be aborted mid operation. Using alternate D addresses has fewer pitfalls.
    The variable I used was the H wear. The part had a tight limit floor depth (+/- 10 microns = 0.0004") and a following shallow angle scanned feature.
    So after the floor and the Z retract, before the start of the scanned feature, I stored the existing H wear offset with a (#150) variable,
    then had the following line with #10004 = 0 (ADJUST Z HEIGHT FOR CHAMFER).
    This tool being T4 (a bull nose - hence me wanting the ability to adjust the Z incase the rad grinding isn't cock-on).
    Then at the end of the feature (T4 toolpaths) on the last line before toolchange, I had this
    #10004 = #150 ( DO NOT CHANGE. THIS LINE POPULATES WEAR TABLE WITH INITIAL SET VALUE FOR THIS TOOL )

    So at the end of the tool, the existing tool wear value is automatically re-entered into the tool table. So next part, the previous H value (whatever that is) is back as was.

  17. #16
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,701
    Post Thanks / Like
    Likes (Given)
    1009
    Likes (Received)
    3220

    Default

    Quote Originally Posted by barbter View Post
    The variable I used was the H wear. The part had a tight limit floor depth (+/- 10 microns = 0.0004") and a following shallow angle scanned feature.
    So after the floor and the Z retract, before the start of the scanned feature, I stored the existing H wear offset with a (#150) variable,
    then had the following line with #10004 = 0 (ADJUST Z HEIGHT FOR CHAMFER).
    This tool being T4 (a bull nose - hence me wanting the ability to adjust the Z incase the rad grinding isn't cock-on).
    Then at the end of the feature (T4 toolpaths) on the last line before toolchange, I had this
    #10004 = #150 ( DO NOT CHANGE. THIS LINE POPULATES WEAR TABLE WITH INITIAL SET VALUE FOR THIS TOOL )

    So at the end of the tool, the existing tool wear value is automatically re-entered into the tool table. So next part, the previous H value (whatever that is) is back as was.
    ^ this is what I meant about careful programming. 👍

  18. #17
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,126
    Post Thanks / Like
    Likes (Given)
    936
    Likes (Received)
    537

    Default

    Quote Originally Posted by Vancbiker View Post
    ^ this is what I meant about careful programming. ��
    Buuuuttt... i was just thinking....If reset got hit after the start of the scanning/chamfer (ie after the second wear H is called) to re-run the tool at the start, then the 2nd wear value will be what's in the tool table...
    Hmmmmm......

  19. #18
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,701
    Post Thanks / Like
    Likes (Given)
    1009
    Likes (Received)
    3220

    Default

    You need to set the appropriate wear value at the beginning of each op.

  20. Likes barbter liked this post
  21. #19
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,681
    Post Thanks / Like
    Likes (Given)
    912
    Likes (Received)
    740

    Default

    To cancel a G43 height offset, you would need a G49.
    Depending on how the machine's parameters are set, BE CAREFUL, I've seen machines "take off" when the offset is cancelled.

    Usually, when I'm done with a tool and send the spindle home with a G28G91Z0;, my startup line after the M06 looks something like this:
    N20 G0 G40 G49 G54 G80 G90 etc

    Now I know that all old offsets and comp are cancelled, cycles are cancelled, etc.


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
  •