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

Sketchucam file doess not mill correctly...help!

Discussion in 'Sketchup Help' started by HuntleyBill, Mar 28, 2017.

  1. HuntleyBill

    HuntleyBill New Member

    Offline
    Messages:
    3
    Trophy Points:
    1
    Location:
    WI
    I am trying out my home built CNC using Sketchucam. I am using GRBL firmware and Universal G-code sender to send the file to the machine. I have made a very simple file to test my CNC. A 30x30 mm cube with 3 tabs. I create the G-code to my desktop. I then use Universal G-Code Sender. I can preview the file. All looks good. I set up the file to mill it in 5 passes. At about 4-1/2 passes the machine becomes possessed and starts milling through the middle of the piece and looks to be re-cutting the piece but doing it offset from the original piece. The preview of the cut path does not show the extra milling operation. So I don't get it. What am I doing wrong?

    I have included a video.
    Thank you for your time!
     
  2. HuntleyBill

    HuntleyBill New Member

    Offline
    Messages:
    3
    Trophy Points:
    1
    Location:
    WI
    Anyone??? Help?
     
  3. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    803
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    @HuntleyBill Please post your sketchup file and the Gcode you generated.
     
  4. HuntleyBill

    HuntleyBill New Member

    Offline
    Messages:
    3
    Trophy Points:
    1
    Location:
    WI
    OK...here is the file. Your advice is appreciated.
    Thank you
     

    Attached Files:

  5. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    803
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    Nothing wrong with the Gcode, so is probably a mechanical problem...
    please reduce your acceleration (to half what they are now) rates for X and Y and run that again. if it then works ok, it means that
    (one or more of)
    a) the accel rate was too high for the power required
    b) something is sticking somewhere, sometimes. (could be chips in the groove loading up the cutter, it is very small)
    c) motor current is too low and could be higher
    d) microstep setting could be reduced which gives more power. (have to adjust steps/mm to match!)

    keen to see a video showing the entire machine, and some more info on the machine itself.
     
  6. TigerPilot

    TigerPilot Well-Known Member

    Offline
    Messages:
    1,576
    Trophy Points:
    48
    I don't use the software that you use so I can't comment on where the UGS software fails, I use Mach3, but you can see in the video where the problem is. On the 5th path it stops at the top right corner, waits a bit, goes up and down and then continues. It looks like it's not going to the tab but stays in the corner, then goes up and down as if cutting the tab and then continues but by then it lost it's spot. As swarfer said, the g-code it perfect so the problem must be in the way UGS interprets the code. If you have the option/access to another software, try it and see if it will work better.

    Just to reiterate, the problem, as swarfer said, is not in SketchUcam. The g-code file is good.
     
  7. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    803
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    actually it is doing 6 passes. you set the material thickness to 5.1mm and the pass depth to 1mm, so the last pass is just .1mm deep. bit of a waste of time (-:
    a possible solution is to do 5 slightly deeper passes
    pass = 5.1/5 = 1.02mm​
    or 6 slightly shallower passes
    pass = 5.1/6 = 0.85mm
    whether you choose bigger or smaller depends on how stiff and powerful the machine is.

    Another thing to look at is feedrate relative to spindle RPM. We want to produce chips rather than dust. Chips tend to fly away while dust tends to pack into the slot. Recutting the dust is very bad for the tool and can also cause the flutes to pack full, then it stops cutting and can even catch fire.
    So, we want to KNOW how big the chips are.
    FR = RPM * T * CL
    Where:
    • FR = the calculated feed rate in inches per minute or mm per minute.
    • RPM = is the calculated speed for the cutter. (or just whatever your spindle does) (note1)
    • T = Number of teeth on the cutter.
    • CL = The chip load or feed per tooth. This is the size of chip that each tooth of the cutter takes.
    For wood, CL is usually 0.05 to 0.25mm but with such a small cutter (you cnc file said 1.7mm) there may not be space in the flutes for bigger chips. So, my router does 24000rpm so I will use that, and assume a 2 flute bit.
    FR = 24000*2*0.1
    = 4800mm/minute​

    wow, fast hey! so, you were feeding at 1800mm/m and that means the chips get smaller, dust, in fact.

    (note1) : rpm is normally calculated from the cutting speed (how fast the tool edge goes past the material) and the diameter of the tool.
    https://en.wikipedia.org/wiki/Speeds_and_feeds
    from that page, for a 1.7mm bit the spindle should be doing 34242RPM at the LOW end of the SFM for wood.

    PS: you should read the SketchUcam manual to learn about the interaction between material thickness and 'overcut%' settings.
    hit the big blue question mark in the toolbar
     
  8. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    803
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    I have just run it through UGS 1.0.9 driving GRBL v1.1f and it completes without error.
     

Share This Page