G68 Coordinate Rotation


Results 1 to 17 of 17

Thread: G68 Coordinate Rotation

  1. #1
    Registered
    Join Date
    Oct 2007
    Location
    USA
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default G68 Coordinate Rotation

    I have this working fine on a Fanuc 16i with one exception. The manual says I can use canned cycles while in this mode, but when I program a G83 for instance, it works fine except that it rapids rather than feeding, and there is no peck. So basically, it makes the move in and out of the hole, but at the rapid feed.

    E.G.
    Coordinate rotation of X about Y on a VMC

    G18 G90 X0 Y0
    G68 X0 Y0 R-45.0
    G91 G83 Z-4.0 F5.0 Q.05 (This moves in the X+, Z- direction at a 45° angle)

    Any help appreciated,

    Thanks,
    Dave

    Similar Threads:


  2. #2
    Member
    Join Date
    Sep 2010
    Location
    Australia
    Posts
    1230
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by DrDave1958 View Post
    I have this working fine on a Fanuc 16i with one exception. The manual says I can use canned cycles while in this mode, but when I program a G83 for instance, it works fine except that it rapids rather than feeding, and there is no peck. So basically, it makes the move in and out of the hole, but at the rapid feed.

    E.G.
    Coordinate rotation of X about Y on a VMC

    G18 G90 X0 Y0
    G68 X0 Y0 R-45.0
    G91 G83 Z-4.0 F5.0 Q.05 (This moves in the X+, Z- direction at a 45° angle)

    Any help appreciated,

    Thanks,
    Dave
    Hi Dave,
    I think you will find that its the G18 that's screwing you over. Change to G17.

    Regards,

    Bill



  3. #3
    Registered
    Join Date
    Oct 2007
    Location
    USA
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default

    The G18 is required to get the rotation I need. Without it, the machine won't move on the correct plane.



  4. #4

    Default

    I think you have to have the G68 in the same block as the G83. Here is an example of a similiar code on a Haas Machine: G72 G Code Explained

    www.WebMachinist.Net
    The Ultimate Online Source for Machinist Related Stuff!


  5. #5
    Member
    Join Date
    Sep 2010
    Location
    Australia
    Posts
    1230
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by DrDave1958 View Post
    The G18 is required to get the rotation I need. Without it, the machine won't move on the correct plane.
    Your example program shows the Centre of Rotation in the X Y plane and your G83 code is in the Z plane. The plane selection should be G17 for your example. If you're wanting to do something other than your example code indicates, then that's something else.

    Regard,

    Bill



  6. #6
    Registered
    Join Date
    Oct 2007
    Location
    USA
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default

    Sorry, let me try to make this clearer.

    My original description was not accurate. The drill cycle line doesn’t drill at all, it merely rapids to the Z depth on that line, moving at the 45° angle. Rapid moves and linear feed moves work great on the rotated plane, just not canned cycles. Here is the current code I'm testing.

    G18 G90 G0 X0 Y0
    G43 H96 Z0.
    G68 X0 Y0 I0. J1.0 K0. R-45.
    S200 M3
    G98 G83 Z-4.0 R0. F50. Q1.0
    G80 G0 Z2.0
    G69
    G17 G90 X0 Y0
    M30

    Attached is a sketch of what I’m trying to do.

    Thanks,
    Dave

    P.S. I'm beginning to think this is a parameter setting. (BTW, I do have parameter 5101.0 set to 1)

    Attached Thumbnails Attached Thumbnails G68 Coordinate Rotation-drilling-using-g68-pdf  


  7. #7
    Member dcoupar's Avatar
    Join Date
    Mar 2003
    Location
    USA
    Posts
    2932
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by DrDave1958 View Post
    Sorry, let me try to make this clearer.

    My original description was not accurate. The drill cycle line doesn’t drill at all, it merely rapids to the Z depth on that line, moving at the 45° angle. Rapid moves and linear feed moves work great on the rotated plane, just not canned cycles. Here is the current code I'm testing.

    G18 G90 G0 X0 Y0
    G43 H96 Z0.
    G68 X0 Y0 I0. J1.0 K0. R-45.
    S200 M3
    G98 G83 Z-4.0 R0. F50. Q1.0
    G80 G0 Z2.0
    G69
    G17 G90 X0 Y0
    M30

    Attached is a sketch of what I’m trying to do.

    Thanks,
    Dave

    P.S. I'm beginning to think this is a parameter setting. (BTW, I do have parameter 5101.0 set to 1)
    Have you tried the G17 per Bill's suggestion?



  8. #8
    Registered
    Join Date
    Oct 2007
    Location
    USA
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default

    Yes, I tried that as soon as I read it. What happens is the machine reverts to the XY plane and therefore drills only moving the Z axis. You must be in G18 mode for both axis to move simultaneously and perpendicular to the rotated plane.

    I'm to the point where I'm going to have to use a macro I found on this site that uses only linear feed moves and rapids to peck drill the hole.
    ...not sure where that leaves me when it's time to tap the holes.

    Thanks,
    Dave



  9. #9
    Member
    Join Date
    Jul 2010
    Location
    South Africa
    Posts
    118
    Downloads
    0
    Uploads
    0

    Default

    you need 1 of the following functions/options,
    3-dimensional coordinate system conversion, A02B-0282-J713 (16i-MB)
    or
    Tilted working plane command, A02B-0282-S676



  10. #10
    Registered
    Join Date
    Oct 2007
    Location
    USA
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by norbert.barnard View Post
    you need 1 of the following functions/options,
    3-dimensional coordinate system conversion, A02B-0282-J713 (16i-MB)
    or
    Tilted working plane command, A02B-0282-S676
    I bought the G68 option back in 2004. It does a 3D rotation properly but the canned cycles don't work. Is this what you mean, or are you talking about something else?

    Thanks,
    Dave



  11. #11
    Member
    Join Date
    Feb 2006
    Location
    india
    Posts
    1792
    Downloads
    0
    Uploads
    0

    Default

    My manual does not show IJK in G68 block???

    Try R45. instead of R-45.

    Edit: I am sorry. R-45. is correct. Counterclockwise rotation is taken positive. One has to view from the positive side of the third axis, y-axis in this case.

    Last edited by sinha_nsit; 01-28-2013 at 11:11 PM. Reason: correction


  12. #12
    Registered
    Join Date
    Jul 2010
    Location
    U.S.A.
    Posts
    104
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by norbert.barnard View Post
    you need 1 of the following functions/options,
    3-dimensional coordinate system conversion, A02B-0282-J713 (16i-MB)
    or
    Tilted working plane command, A02B-0282-S676
    This gentleman says it all. Without this software, your canned cycles are not capable of moving on multiple axes, as indicated by your drawing. You'll need to either purchase the upgrade, or point-to-point program your drilling sequence to accomodate the angle.



  13. #13
    Registered
    Join Date
    Oct 2007
    Location
    USA
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by norbert.barnard View Post
    you need 1 of the following functions/options,
    3-dimensional coordinate system conversion, A02B-0282-J713 (16i-MB)
    or
    Tilted working plane command, A02B-0282-S676
    Thank you Norbert, Fanuc US has confirmed this.

    Dave



  14. #14
    Banned
    Join Date
    Jul 2018
    Posts
    12
    Downloads
    0
    Uploads
    0

    Post Fanuc G68 rotate co-ordinate system for milling program

    Quote Originally Posted by ad64075 View Post
    This gentleman says it all. Without this software, your canned cycles are not capable of moving on multiple axes, as indicated by your drawing. You'll need to either purchase the upgrade, or point-to-point program your drilling sequence to accomodate the angle.
    Fanuc G68 rotate co-ordinate system for milling program
    G68 Command is used to project the operation on an angle .
    G68 command parameters ,
    XY - Center of rotation (co-ordinate used to measure distance )
    R- Angle of rotation (operation projection angle )
    In following fig . we assume corner offset co-ordinate (0 ,0) , In these fig we project the drill of 20 diameter at 45 degree only once a time and depth of drilling is 15 .


    O1423
    N10 M06 T05 ;
    N20 G00 G90 G40 G80 G17 G21 ;
    N30 M03 S1500 ;
    N40 G54 X25 Y0 ;
    N50 M08 ;
    N60 G43 Z100 H4 ;
    N70 G81 Z-15 R5 G98 F300 ;
    N80 G68 X25 Y0 R45 ;
    N90 X50 ;
    N100 X75 ;
    N110 G80 G69 ;
    N120 G00 Z100 ;
    N130 M05 M09 M30 ;
    More examples..........!!!!

    DESCRIPTION OF PROGRAM :_

    O1423- Name of main program
    N10- Tool change command , select tool no 5 ,
    N20- Rapid command , program in absolute co-ordinate ,tool radius compensation cancle , canned cycle command (if we used) , XY plane selection command , metric input ( all dimension in mm)
    N30- Spindle ON clockwise , speed is 1500 rpm .
    N40- Work co-ordinate system command ( set XY value of co-ordinate) , where X25 and Y0
    N50- Coolant is ON
    N60- Tool height offset compensation Z100 and H4(we set tool height of z axis )
    N70- Simple drilling cycle command , drilling depth is -15 , R5 is reference leave (it means tool up 5 mm and then it convert into feed for start next drilling ) , feed rate per minute is F300
    N80- Rotate co-ordinate system command , where X25, Y0 at an angle 45 degree (1st drill)
    N90- Next drill along X distance is 50 .( 2 nd drill)
    N100- Next drill along X distance is 75 .( 3rd drill)
    N110- Cancel canned cycle command , cancel co-ordinate system rotation command .
    N120- Rapid action , tool goes above 100
    N130- Spindle off , coolant off , main program end .

    my link is
    www.hdknowledge.com



  15. #15
    Banned
    Join Date
    Jul 2018
    Posts
    12
    Downloads
    0
    Uploads
    0

    Default

    Fanuc G68 rotate co-ordinate system for milling program example
    August 08, 2018 - FANUC G68 ROTATE COORDINATE SYSTEM [M]

    G68 Command is used to project the operation on an angle .
    G68 command parameters ,
    XY - Center of rotation (co-ordinate used to measure distance )
    R- Angle of rotation (operation projection angle )
    In following fig . we project the drill of 20 diameter at 60 degree six time and depth of drilling is 10.


    O1424
    N10 M06 T05 ;
    N20 G00 G90 G40 G80 G17 G21 ;
    N30 M03 S1500 ;
    N40 G54 X15 Y0 ;
    N50 M08 ;
    N60 G43 Z200 H4 ;
    N70 G81 Z-10 R5 G98 F300 ;
    N80 X15 ;
    N90 X30 ;
    N100 G68 X0 Y0 R60 ;
    N110 X15 ;
    N120 X30 ;
    N130 G68 X0 Y0 R120 ;
    N140 X15 ;
    N150 X30 ;
    N160 G68 X0 Y0 R180 ;
    N170 X15 ;
    N180 X30 ;
    N190 G68 X0 Y0 R240 ;
    N200 X15 ;
    N210 X30 ;
    N220 G68 X0 Y0 R300 ;
    N230 X15 ;
    N240 X30 ;
    N250 G68 X0 Y0 R360 ;
    N260 X15 ;
    N270 X30 ;
    N280 G80 G69 ;
    N290 G00 Z200 ;
    N300 M05 M09 M30 ;

    my linlk is
    http://www.hdknowledge.com/2018/08/f...m-example.html



  16. #16
    *Registered User* andy4035's Avatar
    Join Date
    Jan 2019
    Posts
    2
    Downloads
    0
    Uploads
    0

    Default Re: G68 Coordinate Rotation

    dr dave, curious to know if you could mill a basic profile using this g68 or was it just drilling in linear movements you achieved?



  17. #17
    Registered
    Join Date
    Oct 2007
    Location
    USA
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default Re: G68 Coordinate Rotation

    Quote Originally Posted by andy4035 View Post
    dr dave, curious to know if you could mill a basic profile using this g68 or was it just drilling in linear movements you achieved?
    Been a long time since I used this, but as I remember, the machine acts as it normally would, but with the coordinates rotated. E.G. If you rotated XY 45 degrees, and you simply programmed a Y move, both the X and Y slides would move at a 45 degree angle.

    HTH,
    Dave



  18. #18
    *Registered User* andy4035's Avatar
    Join Date
    Jan 2019
    Posts
    2
    Downloads
    0
    Uploads
    0

    Default Re: G68 Coordinate Rotation

    yes im wondering if i could achieve profiling in and x znd z axis @45deg using this way? I see you could linear drill this way which got me wondering about profiling too.



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 for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

G68 Coordinate Rotation

G68 Coordinate Rotation