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

Y-Axis only goes Right

Discussion in 'Trouble Shooting - Support - Help Section' started by Curt, Jun 17, 2016.

  1. Curt

    Curt New Member

    Offline
    Messages:
    23
    Trophy Points:
    1
    I have a new xpro board and all axis are responding however each time I execute gcode the y axis moves all the way to the right and keeps on going. I have tried multiple times, with different gcode from SketchUcam drawings and each time the same result. X and Z axis seem to be OK.

    I have tried both Grbl-Panel and Grbl Controller, same thing happens.

    Curt
     
    Last edited: Jun 17, 2016
  2. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    807
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    Please post the sketch file and the code file
     
  3. Curt

    Curt New Member

    Offline
    Messages:
    23
    Trophy Points:
    1
    See attached. A simple 5" square with a hole as a test.
    I had to add the *.nc extension in order to upload the gcode.

    Curt
     

    Attached Files:

  4. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    807
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    nothing wrong with the Gcode
    sqc.png
    so, the problem is the hardware:
    Could it be some sort of electrical noise in the wires?
    can you jog Y in both directions?
    can you issue manual (MDI) commands like
    G0 Y100
    G0 Y50
    and have it move both directions? (positive Y is tool moving away, positive X is tool moving right)

    btw you say Y is moving 'right'. left-right is normally X, away/toward is Y. If you set the machine incorrectly the gcode will cut reversed, or crash the tool into something.
    [​IMG]
     
  5. Curt

    Curt New Member

    Offline
    Messages:
    23
    Trophy Points:
    1
    I have nothing odd with the wiring that I can see, although your drawing above told me I had the Y axis running in reversed direction, it is now corrected.

    Yes, I can Jog Y in both directions - as with other 2 axis
    Yes, I can issue manual commands in all directions

    It is a PhlatPrinter III, so unless I got it wrong the X axis is the rollers underneath and the moves the material away in X+, and I have the Gantry as Y axis and moving to the left over the material in Y+ (and my Z moves up vertically in Z+)

    Lines 17/18 is where I have to stop it each time for a run-away Y+ and X+ movement.

    Curt
     

    Attached Files:

  6. Curt

    Curt New Member

    Offline
    Messages:
    23
    Trophy Points:
    1
    OK! Getting closer, I think.

    Suspecting it was a scale issue, I decided to draw a 1" square that was less than an inch from safe zone corner and run the Gcode.

    It ran perfectly, however it is huge and distorted. The 1" square I drew would be cut as an 8.5" x 17"rectangle

    Curt
     
  7. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    807
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    great!
    hmmm, start of a curve, should not be a problem
    in inches, might be a problem but should not be.....
     
  8. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    807
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    ah! scaling, or actually calibration . now we can fix that easily..... (and I never gave it a thought!)

    here I will steal what I wrote on another forum.... and elaborate a little.... (just so I don't have to think up all the math again)

    The formulas are:
    (1) step/mm = stepsperrev / beltpitch / pulleyteeth
    (and a similar one for the leadscrew,...)
    step/mm = stepsperrev / screwpitch​

    and then
    (2) newstep/mm = currentStepPerMM * commandedDist / actualDist

    You use (1) for your initial setup:
    so, for a common setup, a 200 step per rev motor at 16x microstepping, with 3mm pitch belts and 20 tooth pulley
    step/mm = (200*16) / 3 /20
    == 53.33333333 steps per mm (yes, we have to use mm because GRBL works in mm at this level)
    (when calibrating, use as many decimals as you can, it does make a difference)

    then you give a command like (in mm cos GRBL likes it), starting from 0,0
    G21 G0 X20
    X is supposed to move 20mm, but lets say it moves 25mm
    now use formula (2)
    new step/mm = current-step/mm * 20 / 25​

    Replace your current step/mm setting in GRBL with the newly calculated one and it should be 'spot on' depending on how accurately you measured the travel in the first place.
    You can never get more accurate than 1 motor step so don't go chasing hundredths of a mm.

    The higher your microstepping the less accurate it will be, so use the lowest setting that gives you the accuracy you need.
    (cutting foam, do you really need 0.0001" resolution? :)

    Measure over the longest distance possible with your best tool. A plastic dollar store ruler is not good enough.

    Notes:
    1 - since your machine is quite far out, you want to do the basic calculation before the fine tuning, though if you have no idea of the pitch and pulley count you can set steps/mm to "1" and then calibrate twice.
    Now a command like
    G21 G0 Y3200​
    will make the motor above turn once. Measure how far it actually moved the tool and apply formula (2).
    Then do it again (with a shorter movement!) to cross check.

    2 - if ever you change the microstepping, the step/mm value has to be calculated and changed, and recalibrated.

    3 - use the lowest microstepping value that still gives you the resolution you want.
    This will give you the best balance of speed and accuracy.

    4 - on the PP3 none of the XYZ settings will be the same so you have to do each one separately.

    BTW you can run the rollers on the PP3 as X or as Y, just so long as you get all the directions correct (tool movement!), and set 0,0 in the correct place so that G-code works correctly.

    For changing GRBL settings, see this Wiki

    g'night
     
  9. Curt

    Curt New Member

    Offline
    Messages:
    23
    Trophy Points:
    1
    Starting to be fun now.

    So, once I get it cutting the right size (very close now), I can speed it back up I would assume. Getting slower it seems as I lower the steps per mm.

    Thanks for your help, and happy fathers' day to all!

    Curt
     
  10. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    807
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    Yeah, tune speed and acceleration after calibration
    Plenty of web info on tuning, just google it, or even search this forum...
     
  11. Curt

    Curt New Member

    Offline
    Messages:
    23
    Trophy Points:
    1
    Wow, lots of crazy stuff but I am finally understanding things. Incredible how much there is to learn, overwhelming at first but later not all that hard. I now have it calibrated on X and Y, will take on Z next. Played with acceleration and I am learning what things do. So many things to learn and how each tweak affects all other parameters.

    Is there a flow chart somewhere on trimming a CNC machine?
    If not, and if t is possible, maybe someone could create or post a link to one?

    I even learned this weekend how quickly one dollar a sheet "dollar tree foam" clogs up a Phlat printer bit!

    Thank you for your patience with me, a CNC noob

    Curt
     
  12. Curt

    Curt New Member

    Offline
    Messages:
    23
    Trophy Points:
    1
    Oh, and I forgot to say... not only was "Y" going the wrong way, so was X! I did not realize it until I started calibrating and actually put material into the machine (I saw the PP3 rollers rolling away from me in X+ and got fooled into thinking that was correct).

    I am sure more questions will come up as I work with it.

    Having a blast!

    Thanks again,

    Curt
     
    Last edited: Jun 20, 2016
  13. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    807
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    have you googled?
    if the bit is clogging you are probably feeding too fast for the rpm you are running.

    'feeds and speeds' is a big topic in machining, and very important.
    The basics:
    We want each tooth on the cutter to cut a certain amount, say 0.002" 0.002 to 0.015" are common amounts.
    We also want the tooth to travel past the material at a rate that is good for that material. This is known as the surface feet per minute, or SFM.
    SFM varies by material and also by what the cutter is made of, carbon steel vs tungsten carbide vs diamond!? vs ?????
    We want to cut a real chip every time the tooth goes past, no rubbing.
    Each tooth has a gullet into which the chip must fit, if we cut too deep, the chip will not fit = clogging.
    The chips must be thrown clear.
    Multitooth cutters have smaller gullets, so must use smaller chip loads.

    So what numbers to use?
    We can calculate RPM from SFM.
    rpm = SFM * pi / diameter​
    Then we can calculate feedrate from RPM, chipload and tooth count
    IPM = RPM * Chipload * toothcount
    What if our router only has one speed?
    We can still calculate feed speed.
    and, we can fiddle cutter diameter and tooth count to get at least some of what we want.
    ie, to lower SFM use a smaller cutter
    to increase feed speed use more teeth (unless the cutter is small! small cutters have smaller gullets)

    Cutting foam is a little tricky since it is so flexible. So you need to cut 'real chips' but also prevent clogging which might cause melting.
    A tile cutting bit is recommended which is more of a grinder than a cutter. I am sure feedrates for those cutters are mentioned on this forum somewhere, please search.

     

Share This Page