Welcome to Our Community

Some features disabled for guests. Register Today.

What is off on my machine?

Discussion in 'CNC Mills/Routers' started by iH8vols, May 12, 2019.

  1. iH8vols

    iH8vols Well-Known
    Builder

    Joined:
    Dec 4, 2016
    Messages:
    26
    Likes Received:
    4
    Hello.

    I’m trying to cut my first inlay. There’s an endmill toolpath that clears everything and a V-bit path that outlines the image. Both cut their correct paths, however they are not lined up correctly.

    The preview in Aspire is correct so I’m confident it’s not an issue with the toolpath.

    My material isn’t getting shifted. I have a “L” frame setup so that the material is square and the corner of the material is always at the 0,0 home spot.

    Here’s my process.

    1) home and zero everything
    2) drop the pen to the top of the material and zero out the Z axis.
    3) run the endmill toolpath.
    4) move the machine out of the home spot and change pens/bits.
    5) reset the Z axis zero position.
    6) run the V bit path

    Any sound incorrect with this?

    I’ll include a picture of the drawing I did earlier. Red is the endmill path and Green is the V bit path.

    Thanks!
     

    Attached Files:

    Welderben likes this.
  2. jeffmorris

    jeffmorris Veteran
    Builder

    Joined:
    Nov 6, 2017
    Messages:
    225
    Likes Received:
    33
    Did you home, zero everything, and set Z axis zero to top of material after changing bits?
     
  3. iH8vols

    iH8vols Well-Known
    Builder

    Joined:
    Dec 4, 2016
    Messages:
    26
    Likes Received:
    4
    No. I only set the z axis to zero at the top of the material.

    Do I need to rehome/zero the x and y?

    Thanks for responding!
     
  4. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    1,235
    Likes Received:
    616
    please post the gcode file
     
  5. jeffmorris

    jeffmorris Veteran
    Builder

    Joined:
    Nov 6, 2017
    Messages:
    225
    Likes Received:
    33
    Next time you have to change bits, don't move the router/spindle out of home position. Just raise the router/spindle, change bits, and zero Z-Axis at top of material.
     
    iH8vols likes this.
  6. Colin Mccourt

    Colin Mccourt Master
    Builder

    Joined:
    Jan 23, 2019
    Messages:
    346
    Likes Received:
    161
    What I do and it may or may not work for you is when I start a job first home the machine all axis..I then find my datum point in the workpiece whether it be front left or middle. I make a note of the X,Y,Z Co-ordinates.
    Then when I change bits (if you're moving the spindle head) re-cue to X and Y and recalibrate just the Z with.the new bit. Re-set as home position and start the toolpath
    It works for me.
    Regards
    C
     
    iH8vols and GrayUK like this.
  7. iH8vols

    iH8vols Well-Known
    Builder

    Joined:
    Dec 4, 2016
    Messages:
    26
    Likes Received:
    4
    Hey Jeff,

    I just tried this and it worked perfectly. I appreciate the idea because I hadn't thought of that being the issue.

    Is it possible for me to move the bit after Cut 1 to the center of the table to change the bit and then continue with Cut 2? My problem is that my home spot isn't in the best place for me to change bits.

    I'm posting the code if that helps.

    Thanks again. I really appreciate it!
     

    Attached Files:

  8. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    1,235
    Likes Received:
    616
    You don't say what controller you are using but I will assume something GRBL based, but the concepts apply to everything...

    You are running 2 files and between the files you are changing bits.
    Changing bits requires that you change the Z offset. But, at the same time one must not change the X,Y offsets.

    upload_2019-5-14_9-24-40.png
    above is the set of buttons in bCNC that are used for setting work zero.

    After replacing the bit and jogging to the correct height (bit on surface of workpeice?) then one would press the 'Z=0'
    button and never the XY=0 XYZ=0 etc.

    So what are these offsets?
    Every machine has a 'home', this is the physical 0,0,0 point, if it has home switches then they determine this position, if no home switches then this point is wherever the machine got turned on (unless you do something to change it after turn on).
    The convention is the home is at the positive ends of travel.

    Then you have work offsets. This is the offset from home to the 0,0,0 point on the workpeice.
    This is what you are changing when you set zero for the new tool.
    and this is also what must not be changed for X and Y for the new tool.

    Hope this helps
     

    Attached Files:

    Alex Chambers likes this.
  9. jeffmorris

    jeffmorris Veteran
    Builder

    Joined:
    Nov 6, 2017
    Messages:
    225
    Likes Received:
    33
    Home position is usually at left front corner of the machine. What's at that corner that isn't easy for you to change bits?
     
  10. David the swarfer

    David the swarfer OpenBuilds Team
    Staff Member Moderator Builder

    Joined:
    Aug 6, 2013
    Messages:
    1,235
    Likes Received:
    616
    um, no....
    "The convention is the home is at the positive ends of travel."

    Initially this arose because when a moving table milling machine (the first things to be CNC'd) is loaded or unloaded you need the tool high (+Z) and the table all the way forward ( tool is at +Y) and table all the way left (tool is at +X) as the controls are on the right so you need to make space for loading heavy material.

    Due to industrial accidents on machines that were different having tool motion and home in the same place and direction on all machines soon became a convention or standard (and probably law in the EU :) ) . This is why car controls are all the same all over the world.

    We hobby users need to follow these conventions for our own safety and that of our families and guests.

    Yes we need a handy way to position for tool change, that is what G28 and G30 predefined positions are for.
    Provided you always have home in the same place (far right,back,up on my OX) you can jog to where you want to change tools and give a G28.1 and GRBL/Mach/LinuxCNC will remember that place forever. Some GUI's have a button and some you will need to set it on a macro button or just type it like I do.

    I have a friend with a large industrial router and it homes front left. This is infuriating as then the head and gantry are in the way for material loading and since it has a rudimentary control (RZNC501 IIRC) you have to laboriously jog it out of the way everytime you turn it on.
     

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