584,808 active members*
5,180 visitors online*
Register for free
Login
Results 1 to 9 of 9
  1. #1
    Join Date
    Sep 2006
    Posts
    5

    Fanuc tool change homing issue

    I have a Ooya 2185 with a fanuc 15M controller.

    The problem is every time I want to do a tool change I have to make sure it is allways homed in the Z axes. It attemts to do a tool change even when the spindle is 2 inches of the table.

    All the cnc machines I have ever ran you can do a tool change command anywhere and the machine will automaticly move the spindle to the appropriate position and do the tool change.

    Why doesn't T1;M6; work the way I want it too.

    Please help

    Thanks

  2. #2
    Join Date
    Mar 2005
    Posts
    988
    I'd start at the tool change macro. Should be one of the 9000 programs. Probably doesn't have a move in there to back the Z axis out.......

    Although additionaly, I would think that the machine would have some switches in place to check and make sure Z is at the right position before trying to toolchange...
    It's just a part..... cutter still goes round and round....

  3. #3
    Join Date
    Jan 2006
    Posts
    4396
    Why not just write a Tool Change Sub-Program to address the issue for now. Then do more research as to why the machine is doing this.

    O9800
    (ATC)
    G0G40G80M5
    G0G98M9
    G91G28Z0M19
    G0G49G90
    M99
    Toby D.
    "Imagination and Memory are but one thing, but for divers considerations have divers names"
    Schwarzwald

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

    www.refractotech.com

  4. #4
    Join Date
    Dec 2006
    Posts
    84
    Quote Originally Posted by psychomill View Post
    I'd start at the tool change macro. Should be one of the 9000 programs. Probably doesn't have a move in there to back the Z axis out.......

    Although additionaly, I would think that the machine would have some switches in place to check and make sure Z is at the right position before trying to toolchange...

    I would start with the tool change macro also sending it to Z0 before the tool change.

    Not all machines have switches to ensure that it is in position for a tool change. An old Okuma I used to run didn't have any switches. You had to tell it to go to Z0 before changing the tool or it would drop tools.

  5. #5
    Join Date
    Sep 2006
    Posts
    5
    There is nothing in parameter in the 9000's dealing with the tool changer.

    So how do you make a sub program recognize T1;M6;

  6. #6
    Join Date
    Aug 2005
    Posts
    578
    9000 is the program number not a parameter number. It's a protected program.
    On my 0iMc if I MDI a T1 M6, the contents of the 9000 program go by on the screen as it's tool changing

  7. #7
    Join Date
    Mar 2005
    Posts
    988
    As I said (and PBMW restated), a 9000 PROGRAM, not parameter...

    What Toby suggested works too... but it only takes seconds to look at your existing toolchange macro and correct it....
    It's just a part..... cutter still goes round and round....

  8. #8
    Join Date
    Nov 2005
    Posts
    274
    Quote Originally Posted by openforbiz View Post
    I have a Ooya 2185 with a fanuc 15M controller.

    The problem is every time I want to do a tool change I have to make sure it is allways homed in the Z axes. It attemts to do a tool change even when the spindle is 2 inches of the table.

    All the cnc machines I have ever ran you can do a tool change command anywhere and the machine will automaticly move the spindle to the appropriate position and do the tool change.

    Why doesn't T1;M6; work the way I want it too.

    Please help

    Thanks
    You may want to call the MB and find out what they are not doing. The 9000 programs are generally created by the Machine Builder. But you can make a user M code program your self if you want to.

    Go to Parremeter 7080 and put in a value of 616 (M616)

    This will call up program O9020

    O9020(TOOL CHANGE MACRO)
    G0G91G28Z0
    M19
    M6
    M99

    Then anywhere you would use an M6 use M616 this should keep you from crashing untill you can figure out where the 9000 program is for tool change. Some Machine builders have them set up internally and you can not edit them.

    Bluesman

  9. #9
    Join Date
    Dec 2003
    Posts
    24216
    Quote Originally Posted by Bluesman View Post
    Some Machine builders have them set up internally and you can not edit them.

    Bluesman
    Also to stop erasing them accidentally, on the 15M it is P2201 bit #0 = 0 allows editing, set back to a 1 afterwards to prevent accidental erasure.
    Display during execution P2201 Bit1 = 0
    Al.
    CNC, Mechatronics Integration and Custom Machine Design

    “Logic will get you from A to B. Imagination will take you everywhere.”
    Albert E.

Similar Threads

  1. Fanuc 15m Tool Change Problems
    By diggityds in forum Fanuc
    Replies: 11
    Last Post: 12-20-2011, 12:49 PM
  2. Tool change on Fanuc OT
    By steedspeed in forum CNC (Mill / Lathe) Control Software (NC)
    Replies: 5
    Last Post: 09-11-2006, 09:37 PM
  3. Replies: 1
    Last Post: 07-31-2006, 06:19 PM
  4. Homing Issue
    By Moondog in forum Machines running Mach Software
    Replies: 3
    Last Post: 07-30-2006, 04:23 AM
  5. fanuc tool change prompt light
    By cam in forum DNC Problems and Solutions
    Replies: 0
    Last Post: 04-02-2004, 03:27 PM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •