Welcome to Our Community

Some features disabled for guests. Register Today.

Tool Change

Discussion in 'CAM' started by rcKeith, Jun 9, 2016.

Tags:
  1. rcKeith

    rcKeith Well-Known
    Builder

    Joined:
    Jul 1, 2015
    Messages:
    20
    Likes Received:
    15
    Been using sketchucam for a little while and seen the option when you save the parameters for tool change Not to sure how it works and wondered if anyone has used it and what the steps are. I want to drill some small holes in a piece and then switch to a bigger end mill.

    Keith
     
  2. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    799
    Likes Received:
    362
    So you are doing a manual tool change, right?
    and you have read the SketchUcam help on toolchange? it is linked from the 'New i 1.4' section on the front page of the help.

    If you controller understands a 'T1 M6' type of toolchange command, then you can use the first 4 edit boxes to set the parameters for that
    OR
    you use the next 2 edit boxes to set up a macro file and tool offset.

    'tool offset' means that you need to know the difference in length between the first tool and all other tools.
    OR between a 'standard tool' and all other tools. The standard tool can be a spacer that you use between the spindle and the work to set Z-zero. Then all tools have an offset relative to that length.

    You need to write yourself some G-code that matches your machine and the offset system you want to use.
    This code needs to:
    • turn the spindle off
    • position the spindle somewhere for the tool change
    • wait while you change the tool
    • set the tool length offset, or probe for the offset, or ????
    This might look like this
    M05 ; turn spindle off
    G49 ; cancel tool length offsets
    G53 X200 Y0 Z100 ; go somewhere in machine co-ordinates where tool change can be done
    M0 ; wait till resume, NEVER USE a timed delay!
    G43.1 Z21.3 ; the 21.3 is the tool length offset for this tool, as compared to your standard tool
    G0 Z0 ; this may be needed to make sure the tool offset it in effect.​

    In the SketchUcam tool parameters when you specify 'use a tool file' it expects a file like the above code, but with
    G43.1 Z%s
    instead of an offset number.
    The tool length offset you insert in the Tool Offset box will be inserted instead of the '%s'.

    In use, each G-code file for each tool will be generated separately, and then joined using the joiner tool.
    (Gplot will not like the G43.1 line and will not display the code, the basic cut code is going to be fine, but you must test your tool change code very carefully.)

    oh! just spotted a problem in the help example, the G38.1 should be the G43.1 as above. G38.1 is a probe cycle which you can only use if you controller supports it (in the case of GRBL, it does, but the GUI software has to support it as well)

    'standard tool' is usually your longest tool so that all other tools are shorter and thus a negative offset. This provides some safety against crashing in that if you enter the wrong offset, the tool is likely to be too short to hit anything before you figure it out and hit Estop.
    You must set Z-zero using the standard tool

    I have been googling and there is, so far, no good example of using tool changes other than with Mach3 and LinuxCNC.
     
    Joe Santarsiero and Rick 2.0 like this.
  3. rcKeith

    rcKeith Well-Known
    Builder

    Joined:
    Jul 1, 2015
    Messages:
    20
    Likes Received:
    15
    Thanks David that very thorough. I'm using Mach3 so I believe that works OK. I'll give it a try over the weekend.
    I'm trying to make some inrunner brushless mounts for my RC DeHavilland Mosquito. De Havilland Mosquito Had problems on the third flight with motors coming loose even with loctite mainly because there isn't enough material to support tightening the screws. End up with bad takeoff which broke one of the nacelles. So now I have my OX working and a little experience I've decide to build some mounts the hold the motors around the body. Once again thanks for you help.
     
  4. rcKeith

    rcKeith Well-Known
    Builder

    Joined:
    Jul 1, 2015
    Messages:
    20
    Likes Received:
    15
    Hi David
    Can I do a manual zero of the Z axis once its done a move to the tool change area. I tend to use CNCnutz (Peter Passuello) method (Don't spoil your spoil board) method
     
  5. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    799
    Likes Received:
    362
    AFAIK You can only do this if you keep your G-code files per tool separate, ie, do not join them and in fact do not use a tool change macro at all.
    The reason for this is that when the controller is in 'M0' pause mode you cannot jog and set zero.
    Thus you have to set up the tool, then run the Gcode for that tool.

    However, do google the MAch3 manual tool change macro facility.

    Even better, install a tool height sensor (-:
     

Share This Page