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 New
    Builder

    Joined:
    Jul 1, 2015
    Messages:
    24
    Likes Received:
    31
    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 Resident Builder

    Joined:
    Aug 6, 2013
    Messages:
    2,353
    Likes Received:
    1,351
    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 New
    Builder

    Joined:
    Jul 1, 2015
    Messages:
    24
    Likes Received:
    31
    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 New
    Builder

    Joined:
    Jul 1, 2015
    Messages:
    24
    Likes Received:
    31
    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 Resident Builder

    Joined:
    Aug 6, 2013
    Messages:
    2,353
    Likes Received:
    1,351
    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 (-:
     
  6. ADH1234

    ADH1234 New
    Builder

    Joined:
    Apr 23, 2020
    Messages:
    25
    Likes Received:
    4
    Sorry to bring a old thread to life I need some help, I'm new to G-code, learning as I'm going.

    I've created a file on Carbide create as a advanced V carve tool path, which requires a tool change. I'm trying to interpret the g-code to find out how this is done with Openbuilds control. Can someone tell me will the machine pause for a tool change with below G-code at line that reads M0 ;T302 ? if so do I zero z axis and then proceed?



    X23.773Y135.761
    X22.705Y136.684
    X21.739Y137.480
    X20.792Y138.208
    Z12.700
    (Advanced....)
    M0 ;T302
    S10000
    G0X70.589Y519.939
    G1Z-4.445F254.0
    X70.430Y520.153F635.0
    X70.267Y520.459
     
  7. sharmstr

    sharmstr OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Mar 23, 2018
    Messages:
    1,783
    Likes Received:
    1,232
    No. The code wont work with Control. You'll need to create separate files for each tool change. Run the first file, change tools, probe Z only, then run the next file. Rinse and repeat.
     
    Giarc and Peter Van Der Walt like this.
  8. Peter Van Der Walt

    Peter Van Der Walt OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Mar 1, 2017
    Messages:
    9,919
    Likes Received:
    3,164
    Giarc and sharmstr like this.
  9. ADH1234

    ADH1234 New
    Builder

    Joined:
    Apr 23, 2020
    Messages:
    25
    Likes Received:
    4

    I'm relatively new to the CNC and learned on Openbuilds cam but it's limited. Just received my order from openbuilds for some V-bits and playing with them, Carbide create seemed user friendly and recommended through my research. But which of the compatible cams would you suggest? this is a hobbyist/learning experience for me right now and I'd like to stay with the cheaper/ free software.
     
  10. ADH1234

    ADH1234 New
    Builder

    Joined:
    Apr 23, 2020
    Messages:
    25
    Likes Received:
    4
    Appreciate the reply! still a newbie to CNC. so I will do some research on how to separate them, thanks again!
     
  11. Peter Van Der Walt

    Peter Van Der Walt OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Mar 1, 2017
    Messages:
    9,919
    Likes Received:
    3,164
    Then refer to the others, like Fusion 360 - for which our Post also creates seperate tool files for you: docs:software:fusion360 [OpenBuilds Documentation] or Vectric (which has a tickbox for seperate toolfiles in the Toolpath window): docs:software:vectric [OpenBuilds Documentation]


    See docs:software:overview [OpenBuilds Documentation]
     
  12. ADH1234

    ADH1234 New
    Builder

    Joined:
    Apr 23, 2020
    Messages:
    25
    Likes Received:
    4
     
  13. Peter Van Der Walt

    Peter Van Der Walt OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Mar 1, 2017
    Messages:
    9,919
    Likes Received:
    3,164
    Basic entry level CAM software is included yes, but nothing beats the power of a real CAM - its a worthy upgrade - when you want to start doing advanced work requiring toolchanges etc. Then its time to use an advanced CAM as well. We provide posts and support for those too
     
  14. ADH1234

    ADH1234 New
    Builder

    Joined:
    Apr 23, 2020
    Messages:
    25
    Likes Received:
    4
    So I’ve set the toolpaths and used the instructions and added the openbuilds machine in the post processing tab. Everything seems to be in order but I do get this error message. Can you explain?
     

    Attached Files:

  15. Peter Van Der Walt

    Peter Van Der Walt OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Mar 1, 2017
    Messages:
    9,919
    Likes Received:
    3,164
    Yes, you forgot to set a Coordinate system under WCS in the SETUP > Post Process tab How to define Work Coordinate Systems in Fusion 360 Manufacture | Fusion 360 | Autodesk Knowledge Network
    Set it to 0 (first work coordinate system) if you are unsure: 0 = G54, 1 = G55, 2 = G56, 3 = G57 etc - you can layer jobs across multiple coordinate systems (advanced use case, typical for jigging setups)
     
  16. ADH1234

    ADH1234 New
    Builder

    Joined:
    Apr 23, 2020
    Messages:
    25
    Likes Received:
    4
    I’m unsure of what that all means lol.
    It appears it will only accept 1-6 and it says 0 & 1 =g54. So just to confirm I will be ok if I enter the value as 1?
     

    Attached Files:

  17. Peter Van Der Walt

    Peter Van Der Walt OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Mar 1, 2017
    Messages:
    9,919
    Likes Received:
    3,164
    Ahh sorry, yes, correct
     
  18. sharmstr

    sharmstr OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Mar 23, 2018
    Messages:
    1,783
    Likes Received:
    1,232
    When you set it to 1, right click on 1 and click "set as default". Then all new setups will automatically put 1 in there for you.
     
    Peter Van Der Walt likes this.
  19. ADH1234

    ADH1234 New
    Builder

    Joined:
    Apr 23, 2020
    Messages:
    25
    Likes Received:
    4
    any chance someone could review my file?

    after I zero it and run job it dives into the workpiece on the way to the first point of cutting.

    once it got to the first point in drove straight down into the wood and then I aborted the cut.
     

    Attached Files:

  20. ADH1234

    ADH1234 New
    Builder

    Joined:
    Apr 23, 2020
    Messages:
    25
    Likes Received:
    4
    Here is the cut
     

    Attached Files:

  21. sharmstr

    sharmstr OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Mar 23, 2018
    Messages:
    1,783
    Likes Received:
    1,232
    Did you home your machine first? The first move relies on a homed machine. If so, then perhaps you dont have enough clearance for the first move. The first move need 10mm between your stock and your Z limit switch. If you dont have that much clearance, you can try changing your Z start and end position in the post processor properties dialog box to -5.
     
    Peter Van Der Walt likes this.
  22. ADH1234

    ADH1234 New
    Builder

    Joined:
    Apr 23, 2020
    Messages:
    25
    Likes Received:
    4

    Sorry for the questions but can you explain. I did zero the machine on the workpiece before starting and also should have the 10mm clearance. I’m trying to understand the g-code, to me it looks like the first command is to decrease the zaxis -.3937
     

    Attached Files:

  23. Peter Van Der Walt

    Peter Van Der Walt OpenBuilds Team
    Staff Member Moderator Builder Resident Builder

    Joined:
    Mar 1, 2017
    Messages:
    9,919
    Likes Received:
    3,164
    There are multiple coordinate systems
    G53 = Machine Coordinates = set by homing
    G54-G59.1 = Work Coordinates = set by probing and zeroing

    Fusion uses both Machine and Work coordinates

    G53 G0 Z-10 (or Z-0.3937 in inch) means: RAISE Z up to "10mm below the Z homing switch" - as it moves in the G53 coordinate system

    Forgetting to home means moving to "10mm below the switch" looks like a random move, and may even plunge down causing an accident - as G53 (Machine Coordinates) was not established. ALWAYS HOME before setting Work Zero
     
    Alex Chambers and sharmstr like this.
  24. ADH1234

    ADH1234 New
    Builder

    Joined:
    Apr 23, 2020
    Messages:
    25
    Likes Received:
    4
    Great thanks for the information. I’ll give this a try again! Home, work zero and run job :) will let you know if it solved my problem.
     
    Peter Van Der Walt and sharmstr like this.

Share This Page

  1. This site uses cookies to help personalise content, tailor your experience and to keep you logged in if you register.
    By continuing to use this site, you are consenting to our use of cookies.
    Dismiss Notice