Things to include in an M06 macro


Results 1 to 4 of 4

Thread: Things to include in an M06 macro

  1. #1
    Registered
    Join Date
    Nov 2008
    Location
    USA
    Posts
    12
    Downloads
    0
    Uploads
    0

    Default Things to include in an M06 macro

    I've got two cnc mills, the first is a Denford Easimill 3 running Mach3 that I've had for a couple of years. The second is a recently acquired Roadee VMC8 running Flashcut, some of you may have seen the video of this machine when cnccookbook mentioned it:

    http://www.youtube.com/watch?v=l2PWuqgviS8&feature=related]" Automatic Tool Changer" - YouTube

    Both Mach3 and Flashcut use a fanuc style g-code that should be interchangeable. The Denford machine has no toolchanger (yet), but the M06 macro prompts the operator to change the tool, then applies the G43 tool offset. On the VMC8, the G43 & G28 (return to machine home for toolchange) are in the part program and are repeated in the NC file for each toolchange. To me, it seems like these two commands should be part of the macro which would make the tool-change operation self-contained. It would also make the same programs run on either mill without reposting unless there is something else I haven't discovered yet. Is there any reason NOT to do it this way? How does it work on full-size machines? I've only played with hobbyist-type stuff.

    cheers,
    v

    Similar Threads:


  2. #2
    Registered
    Join Date
    Sep 2010
    Location
    Australia
    Posts
    1192
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by vandal968 View Post
    I've got two cnc mills, the first is a Denford Easimill 3 running Mach3 that I've had for a couple of years. The second is a recently acquired Roadee VMC8 running Flashcut, some of you may have seen the video of this machine when cnccookbook mentioned it:



    Both Mach3 and Flashcut use a fanuc style g-code that should be interchangeable. The Denford machine has no toolchanger (yet), but the M06 macro prompts the operator to change the tool, then applies the G43 tool offset. On the VMC8, the G43 & G28 (return to machine home for toolchange) are in the part program and are repeated in the NC file for each toolchange. To me, it seems like these two commands should be part of the macro which would make the tool-change operation self-contained. It would also make the same programs run on either mill without reposting unless there is something else I haven't discovered yet. Is there any reason NOT to do it this way? How does it work on full-size machines? I've only played with hobbyist-type stuff.

    cheers,
    v
    Tool Change Macro Programs are many and varied. Some MTB use the Macro Programs to read Interface Inputs to determine the state of various proximity switches so that the position of the various components of the Tool Change mechanisms are known, other do all this work in the PLC (PMC) program. Some Tool Change programs are merely used to automate the process of getting the spindle etc in the right place for the tool change to occur, for example, making sure that the spindle is at the correct height for the tool change by using G28 or G30.

    As your machines use a manual tool change process, its probable that the Macro program only needs to position the spindle to a safe and convenient position to execute the manual change. G43 is the code to apply the Tool Length Offset in a + direction. I can't see that being required in a Tool Change Macro, particularly when G28 (Reference Return via an Intermediate position) is used. Its more common practice to use G43 in conjunction with the current tool's Tool Length Offset, and during a move command after the tool change has been completed. For example:

    G43 Z10.0 (mm) H02

    If, like a Fanuc control, your machine has G53 available, this is often used to define a safe and convenient XY coordinate position for the tool change. I believe that a machine that uses a Manual Tool Change process would only need code to ensure that:
    1. the Spindle is stopped M05
    2. the spindle is in the correct position in Z for the tool change G91 G28 Z0.0
    3. the spindle is in a convenient position in X and Y for the tool change G53 X_ Y_
    4. a compulsory stop command is used to halt the program M00
    5. a message is displayed to prompt the operator to take action. Again, if the programming and Macro syntax is similar to a Fanuc, a message is raised by #3006=1 (CHANGE TOOL). With a Fanuc control, this command also halts the program similar to M00.

    Regards,

    Bill

    Last edited by angelw; 05-07-2012 at 08:07 PM.


  3. #3
    Gold Member
    Join Date
    Feb 2009
    Location
    usa
    Posts
    5794
    Downloads
    0
    Uploads
    0

    Default

    We just assign M6 to a 8000 Macro. Since the builders M6 controls pretty much everything, ours simply returns Z to the G28, calls factory M6 and returns. On the small machines, they may move the table out of the way as well.



  4. #4
    Registered
    Join Date
    Nov 2008
    Location
    USA
    Posts
    12
    Downloads
    0
    Uploads
    0

    Default

    Thanks for the help guys.

    cheers,
    v



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

Things to include in an M06 macro
Things to include in an M06 macro