Using Fanuc's G28


Results 1 to 6 of 6

Thread: Using Fanuc's G28

  1. #1
    Registered tahlinc's Avatar
    Join Date
    May 2003
    Location
    Tucson, AZ USA
    Posts
    70
    Downloads
    0
    Uploads
    0

    Default Using Fanuc's G28

    Mike Lynce at http://www.cncci.com/ helped me understand this.

    What he taught me was:
    G28 is a two part command.

    First part is a rapid move to the coordinate location included with the command in the current coordinate system. This is an intermediate position.

    The 2nd part is a rapid move (all at once) to machine zero for the same coordinates listed.

    The simplest use of this command is to return Z to machine zero for tool change after making the preparatory move. Since only a move in Z is desired, Z is the only axis listed. Since we do not want the machine to move in Z during the preparatory we use G91 G28 Z0. We could also have used G91 G28 Z.1 that would first rapid up 0.1 then rapid to machine zero. Using Z0 is just simpler.

    This command does introduce G91 so be sure to call G90 afterward.

    Another use would be to rapid to machine zero in three axis at once (ouch!). First get away from every thing then rapid in all three axis to machine zero.

    G91 G28 X0 Y0 Z4

    This helped me.
    Cheers,
    Jim
    www.tahlcam.com

    Similar Threads:


  2. #2
    Member Paul_S's Avatar
    Join Date
    Mar 2003
    Location
    Mira Loma, California
    Posts
    156
    Downloads
    0
    Uploads
    0

    Default G28 G53

    I program Fadal mills. And they use the G28 different than the Fanuc format. Absoute mode and the code by itself.

    N1G28 (typically)

    We also have one Haas mill which follows the Fanuc format. But since the code G91G28X0Y0Z0 sends the machine spindle to the far right hand machine home position, I do not like to use it.

    Instead I use the machine coordinate system command G53.

    (first program blocks)
    G90G53Z0
    G53X-15.Y0 (machine has a 30 inch X axis travel)

    (last program blocks)
    G53X-15.Y0
    G0G90G40G80T1M6
    M30

    Safety - Quality - Production.


  3. #3
    Registered Rekd's Avatar
    Join Date
    Apr 2003
    Location
    teh Debug Window
    Posts
    1876
    Downloads
    0
    Uploads
    0

    Default Re: G28 G53

    Originally posted by Paul_S
    I program Fadal mills. And they use the G28 different than the Fanuc format. Absoute mode and the code by itself.

    N1G28 (typically)

    We also have one Haas mill which follows the Fanuc format. But since the code G91G28X0Y0Z0 sends the machine spindle to the far right hand machine home position, I do not like to use it.

    Instead I use the machine coordinate system command G53.

    (first program blocks)
    G90G53Z0
    G53X-15.Y0 (machine has a 30 inch X axis travel)

    (last program blocks)
    G53X-15.Y0
    G0G90G40G80T1M6
    M30
    The fadal can run either format. If you set it to FORMAT 2 (been years, I think it's 2), it will act more like the HAAS, including G54 offsets instead of E1.

    You can change the HAAS code and remove the X move so it won't move the table all the way over.

    'Rekd

    Matt
    San Diego, Ca

    ___ o o o_
    [l_,[_____],
    l---L - □lllllll□-
    ( )_) ( )_)--)_)

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  4. #4
    Member Paul_S's Avatar
    Join Date
    Mar 2003
    Location
    Mira Loma, California
    Posts
    156
    Downloads
    0
    Uploads
    0

    Default Format 1

    Yes, Fadal format 2 is the Fanuc format on the Fadal. But I prefer not to use it, if I don't have to.

    Some codes are not supported. G9 default on the Fadal is what is called a G61 on the Fanuc control. But the default Fanuc G64 milling mode code is equal to the G8 on the Fadal. But G64 & G61 is not supported in the Fadal Fanuc format 2.

    Also using the Fadal format I don't need to use G43 with the H word or the D word with G41 or G42.

    The Fanuc format only supports fixture offsets G54-G59 (same as the Fadal E1-E6.) The Fadal format uses E1 through E24. The Haas uses after G59, G110, G111, G112 etc.

    The Mark Century 2000 control uses both G54-G59 fixture offsets along with E1-E24. So when I programmed that control I used G54 to set one program zero. And used the E offsets 1-8 for all
    the others from the G54 offset. Was like having multiple G52 offsets except the E offsets had to set and pickup just as one would the G54-G59.

    Safety - Quality - Production.


  5. #5
    Registered tahlinc's Avatar
    Join Date
    May 2003
    Location
    Tucson, AZ USA
    Posts
    70
    Downloads
    0
    Uploads
    0

    Default Re: G28 G53

    Originally posted by Paul_S
    But since the code G91G28X0Y0Z0 sends the machine spindle to the far right hand machine home position, I do not like to use it.
    M30
    Yes I see the problem. If you leave out the X and Y it will only home the Z.

    G53 is great but not all Fanucs have it.



  6. #6
    Registered
    Join Date
    Mar 2008
    Location
    USA
    Posts
    2
    Downloads
    0
    Uploads
    0

    Default machinist

    Use of G28 commands vary from situation to situation. We have some older Motch/Merryweather turret lathes that have a pretty old Fanuc control that has only one offset table, no wear offsets. The only way to ZRN a tool in that situation is to retract the tool to a safe distance, WITHOUT a command to clear the offset, then G28 G91 X0 Z0. If you clear the offset first, the tool will physically repostion itself by the distance equal to the offset's value, which would be the tool's true lengths (X and Z on a turret lathe), possibly resulting in a crash.
    On the newer Fanucs, which have wear AND Geometry offsets, The first execution of the G28 command (in G91 mode) physically repositions the tool by an amount equal to the values in the wear offset (usually only a few thousandths inch). The second execution of the G28 command in G91 mode (incremental mode) sends the tool to it's ZRN position. I noted the presence of G91 mode during this command because it is possible to execute a G28 command while in G90 mode (absolute mode). The results of this would be the positioning of the tool, in rapid traverse, to the center of the chuck in X axis and to the Programmed Z zero point, which never ends happily if there's a workpiece in the tool's way.
    BUT, this is not always the case, depending on which G code group is being applied. We just got a new 3 axis vertical lathe (X, Z, and C) up and running this week that uses G code Group "A". In this setting, G28 U0 W0 H0 works the same way as the 2 step execution described above with Wear offsets ("U" for X axis, "W" for Z axis, "H" for C axis).



Tags for this Thread

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

Using Fanuc's G28

Using Fanuc's G28

Using Fanuc's G28