1. Hey guyz. Welcome to the All New Phlatforum!

    Sign Up and take a look around. There are so many awesome new features.

    The Phlatforum is a place we can all hang out and

    have fun sharing our RC adventures!

  2. Dismiss Notice

g-code joiner

Discussion in 'General Talk Forum' started by john bell, Apr 17, 2017.

  1. john bell

    john bell New Member

    Trophy Points:
    I want to work on a project which involves using different bits. I understand that one can use the g-code joiner and have the ability to change bits for different portions of the job. I've gone to the help section which I didn't understand, and tried to find a video explaining the process but couldn't find anything. Does anyone know of a source which gives a good explanation?
  2. swarfer

    swarfer Moderator Staff Member

    Trophy Points:
    Grahamstown, South Africa
    The help IS the source (-: (so far)

    Assuming you do not have a controller that can do 'T3 M6' type tool changes.....

    what controller are you using, and if GRBL, what GUI?
    some support toolchanges so maybe you want to try one of those (like bCNC)

    In SketchUcam you need to enable the Quicktools toolbar so you can access the tool change tool (the big T).
    In Sketchup, activate this toolbar by ticking the `View|Toolbars|SketchUcam Quick Tools` item.

    You also need to set up a toolchange macro. There are some in the help:
    the first one is this (which is the easiest to use)
    M5  (stop the spindle)
    G49 (turn off offsets)
    G28 (go to predefined position)
    M0 (pause for tool change)
    G43.1 Z%s 
    (toolchange end)
    before using that you need to make sure the G28 is set to a place where it is safe to change tools and the tool will not crash into the work on the way to the G28 co-ordinates.
    make sure the G43.1 line is just as above, with only one %s in it

    You need to save your chosen macro into a file, mine is called toolchange.nc

    Now, in SketchUcam when you click the T tool in the Quicktools toolbar you get this
    make sure Tool number is -1
    'tool file' is normally 'no' the first time you do this, set it to yes
    set the offset for this tool, this is the number that will be inserted in the line
    G43.1 Z%s
    which will tell GRBL how much this tool differs from the first one.
    click ok, and you will be prompted for the toolchange macro file.

    Now in Sketchup click the T and fill in the offset for the first tool, normally 0
    select the drawing that must cut with this tool
    generate Gcode to 'tool1.nc'

    click T and fill in the offset for tool 2
    select the drawing that must cut with this tool
    generate Gcode to 'tool2.nc'

    click T and fill in the offset for tool 3
    select the drawing that must cut with this tool
    generate Gcode to 'tool3.nc'

    now join those 3 together and do a TEST cut with no tool and plenty of room for error and a nervous finger on the Estop button (-:

    I will make a note to make a video about this....

Share This Page