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
Welcome to The Phlatforum PhlatPrinter III

Circles: Feed Rate Slows

Discussion in 'SketchUcam Help' started by phlatfoot, Sep 4, 2014.

  1. phlatfoot

    phlatfoot New Member

    Offline
    Messages:
    15
    Trophy Points:
    1
    Hope I'm not asking a question answered elsewhere -- I did a forum search first...

    I'm using Sketch-U-Cam 1.1D and Sketchup 7.1, and cutting with TurboCNC.

    I tend to increase the number of segments in circles and arcs in Sketchup to 50 to avoid the faceted look. But this really slows down the feed rate because of the acceleration factor in TurboCNC. The segments are so short that the stepper never reaches the feed rate, or even remotely close to the feed rate.

    Seems like there are probably two solutions -- either hand program circles to use a proper G-code rather than a circle composed of segments out of SketchUP. Or turn off acceleration in TurboCNC -- but that would mean reducing the max feed rate -- I think. Not sure -- new to this.

    Am I just missing a solution in SketchUp or Sketch-U-Cam?

    Oh also somewhat related question -- are tabs shortened in sharp curves/circles due to the short segments -- it seems like they act that way....

    Thanks!
     
    phlatfoot, Sep 4, 2014
    #1
  2. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    for plain circles and arcs (that you don't edit) SketchUcam will output true G2/G3 arcs segment codes. so no matter that it look ssegmented in the screen view, the Gcode will be true arcs.

    The moment you edit an arc it may become line segments. experiment and see what works for you.
    with short segments you can just drag the tab tool along several of them to get a 'long enough' tab on the arc.
     
    swarfer, Sep 4, 2014
    #2
  3. phlatfoot

    phlatfoot New Member

    Offline
    Messages:
    15
    Trophy Points:
    1
    Ahhhh, thanks very much Swarfer!
     
    phlatfoot, Sep 4, 2014
    #3
  4. phlatfoot

    phlatfoot New Member

    Offline
    Messages:
    15
    Trophy Points:
    1
    Hmmm -- you've got me thinking about where I might be editing the circles -- I wonder if specifying 50 segments is the place where that is happening. Ironic if it is, since I'm trying to smooth them in the cut!

    I'll do some tests to check it out. Thanks a
     
    phlatfoot, Sep 4, 2014
    #4
  5. phlatfoot

    phlatfoot New Member

    Offline
    Messages:
    15
    Trophy Points:
    1
    I just did a test for two circles, and it actually outputs a G3 but repeats it for each segment -- in other words it treats a 25 segment circle as 25 arcs. TurboCNC applies the acceleration factors to each arc individually, so ramps up for each arc. Of course it never reaches feed speed in a small circle and the net effect is the the circle is cut at a very slow feed rate.
     
    phlatfoot, Sep 4, 2014
    #5
  6. 3DMON

    3DMON Moderator Staff Member

    Offline
    Messages:
    2,380
    Trophy Points:
    38
    Location:
    Sebastian, Florida
    This seems odd because Mach3 sees the G3/G2 codes just fine.
    In Sketchup it shouldn't matter how many line segments as long as the circle or arc stays whole when highlighted. If you click on it and it only highlights a segment of the arc or circle that's where the problem is.
    I'm not familiar with TurboCNC but maybe there is a setting in it that is off for the G2/G3 commands.
     
    3DMON, Sep 5, 2014
    #6
  7. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    then you want FEWER segments (-:
    <theory> for simple arcs it should be possible to output a single G2/3 command for the entire arc. The problem is that the moment the arc gets edited Sketchup does some weird internal things causing the edited ends of the arcs to be problematic when you translate them into Gcode. biggest problem is telling the difference between plain arcs and edited arcs, I have not found a way to do it.

    TurboCNC is very long in the tooth now and really does not support Gcode all that well. I say this because the solution to this issue is the G64 command, which tells a controller to maintain speed through corners at the expense of some precision. For 'corners' read 'joints of the arcs'.
    LinuxCNC supports the extra parameter to G64, telling it just how much precision you want. So you can tell it to maintain speed if it can keep within 0.25 or 0.5mm of the programmed path. On segmented arcs, 0.25mm is small enough that you cannot feel it, but it will maintain speed through the intersections as though it were one long arc. I believe Mach3 also supports this command.

    Downside of more modern software is that you need a bit more oomph in the motherboard. A P4 2.4Ghz with 2GB or RAM will work fine though, so long as you do not put a large high resolution screen on it without also putting in a 'better then the onboard' graphics card in it. I've got such a machine right here (-:

    I have not spotted a USB based controller that supports G64, yet.....
     
    swarfer, Sep 5, 2014
    #7
  8. phlatfoot

    phlatfoot New Member

    Offline
    Messages:
    15
    Trophy Points:
    1
    Thanks for your advice guys!

    FYI, there was no editing of the test circles I tried -- SketchUP always treats these as arc segments for the number of default segments it is running with. Sketch-U-Cam does write these as multiple arcs in G-code, following suit. But it does not do more than that.

    I had already decided to try out LinuxCNC a couple days ago since I realized the fault was in TurboCNC lacking a lookahead buffer and compensation for speed. Puppy Linux is my main OS anyway. (which is why I wasn't running Mach3.) so I was used to Linux.

    TurboCNC was running fine for years on a 1998 Pent 3 Thinkpad 600E laptop (despite occasional web recommendations against laptops).

    Out of curiosity I checked the latency on the Thinkpad, and it was surprisingly good. So I bit the bullet and ran LinuxCNC from live disk (older Ubuntu 8.04 edition), and that worked, too, though the OS was slow.

    So I Installed it to HD so I could dual boot back to my other onboard OS's (yes several!) and it seemed to work well in simulation. Finally with all parameters loaded for my gantry mill I did some experimental foam cuts. All went well, so I tried 14 ga. aluminum -- it also worked. Feed speeds were proper (had to be for aluminum) so I'm good to go.

    I don't like Ubuntu, too slow and bloated as an OS, but this is a dedicated controller, so it doesn't matter, as long as the CNC program runs well. Starting programs or opening windows has me tapping my fingers and yawning. But it cuts good!
     
    phlatfoot, Sep 8, 2014
    #8
  9. 3DMON

    3DMON Moderator Staff Member

    Offline
    Messages:
    2,380
    Trophy Points:
    38
    Location:
    Sebastian, Florida
    So it was just a TurboCNC issue. Glad to hear things are working for you now.
     
    3DMON, Sep 8, 2014
    #9
  10. swarfer

    swarfer Moderator Staff Member

    Offline
    Messages:
    808
    Trophy Points:
    28
    Location:
    Grahamstown, South Africa
    great! note that LinuxCNC will run through a network with X forwarding, so you don't actually have to run the GUI on the laptop.
    I run Ubuntu Studio on my main machine, and the recent 'upgrade' to Unity desktop sucks. My son has Xubuntu, the one with XFCE, which is much sticker. If you can unload Unity and load XFCE instead you will be much happier with Ubuntu, just be sure not to disturb the realtime kernel.

    The warnings against laptops are mostly to do with most newer laptops running the parallel port at 3.3 volts instead of 5 volts. This causes problems for our stepper drivers unless we make sure to drive 'active low' AND the port has open collector outputs.
     
    swarfer, Sep 9, 2014
    #10

Share This Page