Fanuc 18m toolchange macro program (dahlih mcv 720)
Close
Login to Your Account
Results 1 to 6 of 6
  1. #1
    Join Date
    Apr 2021
    Country
    SOUTH AFRICA
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Fanuc 18m toolchange macro program (dahlih mcv 720)

    Hi Everyone

    I'm hoping someone will be able to help me. I I have a Dahlih MCV 720 (1999 model) with a Fanuc 18M controller.

    The machine has lost it's PARAMETERS, fortunately I had a backup a got it loaded and machine is working.however I canít change tools as the macro program was lost. Iím hoping someone will b able to help me with the tool change macro program or point me in the right direction.
    Any help will b much appreciated.


    Please let me know if there is any other info I can provide.

    Thanks.

    regards
    Bashier

  2. #2
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,086
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1720

    Default

    Quote Originally Posted by Akaz View Post
    Hi Everyone

    I'm hoping someone will be able to help me. I I have a Dahlih MCV 720 (1999 model) with a Fanuc 18M controller.

    The machine has lost it's PARAMETERS, fortunately I had a backup a got it loaded and machine is working.however I canít change tools as the macro program was lost. Iím hoping someone will b able to help me with the tool change macro program or point me in the right direction.
    Any help will b much appreciated.


    Please let me know if there is any other info I can provide.

    Thanks.

    regards
    Bashier
    Hello Akaz,
    I haven't got a copy of the Tool Change Macro for your particular machine, but can you describe what happens when you attempt a tool change?

    Tool change can be carried out completely by the PMC Program, or by a combination of User Macro and PMC Program; its up to the MTB as to how this is accomplished. If the Tool Change is executed by the PMC, it could be a case of a Tool Change Macro doing no more than ensure that the Z Axis (vertical machine) is in the correct position for a Tool Change. Accordingly, knowing what occurs now when you attempt a Tool Change may point to how a Tool Change Macro assists and a new Tool Change Macro may be able to be reconstructed.

    If the above approach fails and you have no joy with someone on the Forum reaching out to you with a copy of the Tool Change Macro, your best bet would be to contact the agents in your country for your machine, or directly to the MTB. In either case, supply the Serial Number and build date of the machine with your request for a copy of the Tool Change Macro.

    Regards,

    Bill

  3. #3
    Join Date
    Apr 2021
    Country
    SOUTH AFRICA
    Posts
    2
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Hi Bill

    When the machine reads M6 it gives a alarm (078 number not found)

    Iíve had I few technicians out and all tell me I need the specific macro program.

    If I do the tool change in single block as manual says u can, it works.
    However those commands donít work in memory mode which the manual also says.

    I have emailed the Agents/manufacturer and have had no reply.

  4. #4
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,086
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1720

    Default

    Quote Originally Posted by Akaz View Post
    Hi Bill

    When the machine reads M6 it gives a alarm (078 number not found)

    Iíve had I few technicians out and all tell me I need the specific macro program.

    If I do the tool change in single block as manual says u can, it works.
    However those commands donít work in memory mode which the manual also says.

    I have emailed the Agents/manufacturer and have had no reply.
    Hello Akaz,
    Would you mind Posting the commands you used in your single block exercise?

    Regards,

    Bill

  5. #5
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    757
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    267

    Default

    It sounds like you're missing a 9000 series tool change Macro/Subroutine. In Memory or Auto Mode, when the control sees an M code, it first looks to see if there is a Macro or Subroutine assigned to that number. If not, it then goes on to the PMC and works through what it finds there. That might be why you get a "Number Not Found" alarm in Auto and it works in MDI. (Which I believe was called Single Block by mistake)

    Look at parameters 6071 thru 6089 and see if you find a 6 next to one of them. If you do, that parameter tells you what the Tool Change program/macro number has to be. Below is a generic tool change routine that I've used on more then one Fanuc machine without trouble. Store it in your control but change the 9001 number to match whatever you find in your parameters.

    Parameter 6071 links to a Subroutine numbered 9001 which is your most likely suspect.
    It goes on in an orderly fashion from there.
    6072 - 9002
    6073 - 9003
    ...
    ...
    ...
    6079 - 9009

    Starting at Parameter 6080 (link 9020) they turn into Macros.
    6081 - 9021
    ....
    ...
    ...
    ...
    6089 - 9029

    (Note: Parameter 3202.4 (NE9) will temporarily have to be set to 0 for the control to accept the new 9000 series program. Turn it back to 1 when you're done.) After changing NE9, do a quick double check of your program list and make sure you're not going to overwrite anything. Not likely, but I always do double and triple takes when monkeying with parameters.

    %
    O9001 (M6 TOOL CHANGE)

    G0G80G40M9
    G91G28Z0M5
    M19
    M6
    G90
    M99
    %

    I know... M6 calling a sub that calls M6, sounds crazy but it works.

    It wouldn't surprise me if angelw can ultimately supply you with a more elegant solution, but this will likely get you going.

  6. Likes PROBE liked this post
  7. #6
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,086
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1720

    Default

    Hello Akaz,
    If your Tool Changer is the variety that can have the next tool called to the ready position, the Tool Change Program will most likely be called as a Macro Program, rather than a Sub Program. Accordingly, if you look at parameters 6080 through 6089 for the registration of the number 6, that will at least tell you the number of the Macro Program that's missing. Program numbers O9020 through O9029 relate respectively to parameters 6080 through 6089.

    If the Tool Change Program is called as a Subprogram, look in parameters 6071 to 6079 for the registration of the number 6 to determine the program number being called. Program numbers O9001 through O9009 relate respectively to parameters 6071 through 6079.

    The issue with reconstructing a Tool Change Macro from scratch, is if there is interaction between the Macro Program and the PMC; the Macro Program being held up until the particular status of a proximity switch is communicated to it by the PMC for example; that's the reason I'd like to see the commands you use in your successful operation of the Tool Changer in Single Block.

    Regards,

    Bill


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
  •