Leadwell v-40 m6 subprogram accidentally deleted
Close
Login to Your Account
Likes Likes:  0
Results 1 to 7 of 7
  1. #1
    Join Date
    Oct 2020
    Country
    FINLAND
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Leadwell v-40 m6 subprogram accidentally deleted

    Hello machinist fellas

    I accidentally deleted programs numbered 9000-9004. I'm in trouble now because M6 won't change tools now. When i try to change tool with m6, alarm "078 NUMBER NOT FOUND" appears and nothing happens. I dont have any manuals and no idea, how to write that again. Machine is Leadwell V-40 with Fanuc Series 21-M panel. This question might sound stupid but I'am student. And yes, my teacher dont know neither.

    Thanks already
    Sirkuskissa

  2. #2
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,979
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1637

    Default

    Quote Originally Posted by sirkuskissa View Post
    Hello machinist fellas

    I accidentally deleted programs numbered 9000-9004. I'm in trouble now because M6 won't change tools now. When i try to change tool with m6, alarm "078 NUMBER NOT FOUND" appears and nothing happens. I dont have any manuals and no idea, how to write that again. Machine is Leadwell V-40 with Fanuc Series 21-M panel. This question might sound stupid but I'am student. And yes, my teacher dont know neither.

    Thanks already
    Sirkuskissa
    Hello Sirkuskissa,
    First, look at bit 5 of parameter 6001. If set to 1, Program O9000 will be called by a "T" code. This program will normally only apply to a Umbrella type tool changer where each tool can only reside in respective individual pockets. This type of system doesn't actually require an M06 to carry out a tool change. If bit 5 is set to Zero, you can disregard program O9000 for the moment.

    For programs O9001 through O9004, look in the corresponding parameters 6071 through 6074 for the registration of the numeral "6". Whichever parameter in that range of 6071 through 6074, has 6 registered, will call the respective program O9001 through O9004. Lets say that 6 is registered in parameter 6072, then program O9002 will be called when M06 is executed in a program. In this case, if you were to register a program in memory under the number O9002 as follows:

    O9002
    M99

    then the issue of the "078 NUMBER NOT FOUND" alarm would be resolved, but no tool change would occur. You really need to know the content of the program that's was being called by M06.

    The Tool Change of any Fanuc controlled machined can be totally carried out by the PLC (PMC in Fanuc Speak), or by a combination of program commands and the PMC. The Tool Change Macro being called by M06 may be no more than ensuring the Z axis is at Reference Return and the X/Y axes are in a safe location for a Tool Change to occur, or it could cater for a more complex interaction with the PMC.

    If you don't have a copy of the 9000 series programs, I'd suggest that your best action would be to contact the local agent and or machine builder of the machine, stating the serial number of the machine.

    Regards,

    Bill

  3. #3
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    1,444
    Post Thanks / Like
    Likes (Given)
    660
    Likes (Received)
    856

    Default

    For the future I believe 3202.4 will prevent editing of 9000 series programs

  4. #4
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    3,259
    Post Thanks / Like
    Likes (Given)
    1320
    Likes (Received)
    1410

    Default

    Contact Leadwell or their local-ish distributor to get it. If an email doesn't work then try by phone, or phone first. They will want the serial # of the machine.

  5. #5
    Join Date
    Feb 2008
    Location
    MI, USA
    Posts
    915
    Post Thanks / Like
    Likes (Given)
    70
    Likes (Received)
    376

    Default

    What year and serial is your leadwell?

    This is from a 1999 machine, "series no L1SIH037"

    The front is square/boxy rather than some models (cant remember which year) that are curved.

    If your machine is older or newer, it may still work, but I can't guarantee the ladder and counters are the same.




    :9001
    M6T#4120
    #1132=0
    IF[#1012EQ1]GOTO60
    M66
    IF[#1008EQ1]GOTO60
    G80
    #130=#4003
    #131=#4006
    G91G28Z0
    G49
    IF[#1013EQ0]GOTO60
    #1102=1
    N10IF[#1009EQ0]GOTO10
    G30Z0
    N30IF[#1010EQ0]GOTO30
    G28Z0
    #1132=0
    G#130
    G#131
    N50IF[#1011EQ0]GOTO50
    N60M67
    M99


    Also, as a side note, you should really just tell the teacher. I'm sure the guy has program backups to the machine. or at least he should...

  6. #6
    Join Date
    Oct 2020
    Country
    FINLAND
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I found backup program and i changed the delete protect parameter for 9000 programs. Thanks for the help guys!

    -Sirkuskissa

  7. #7
    Join Date
    Oct 2020
    Country
    FINLAND
    Posts
    6
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by dandrummerman21 View Post
    What year and serial is your leadwell?

    This is from a 1999 machine, "series no L1SIH037"

    The front is square/boxy rather than some models (cant remember which year) that are curved.

    If your machine is older or newer, it may still work, but I can't guarantee the ladder and counters are the same.




    :9001
    M6T#4120
    #1132=0
    IF[#1012EQ1]GOTO60
    M66
    IF[#1008EQ1]GOTO60
    G80
    #130=#4003
    #131=#4006
    G91G28Z0
    G49
    IF[#1013EQ0]GOTO60
    #1102=1
    N10IF[#1009EQ0]GOTO10
    G30Z0
    N30IF[#1010EQ0]GOTO30
    G28Z0
    #1132=0
    G#130
    G#131
    N50IF[#1011EQ0]GOTO50
    N60M67
    M99


    Also, as a side note, you should really just tell the teacher. I'm sure the guy has program backups to the machine. or at least he should...
    I already told the teacher but he couldn't help me so I asked from you guys. That program you sent is correct


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
  •