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

Corners cutting round

Discussion in 'EMC' started by cncmachineguy, Mar 30, 2010.

  1. cncmachineguy

    cncmachineguy Member

    Offline
    Messages:
    133
    Trophy Points:
    16
    Location:
    Odenton MD
    Hi Guys,

    Rosie seems to cut her corners round. Now I don't mean the 1/16 radius left from the cutter, I mean like 1/4" radius. It seems like she is not finishing her cut in 1 direction before starting the turn. Maybe I have my accel/decel wrong, but I am wondering if anyone knows of a setting somewhere to force the line execution of each line before starting the next.

    To me, this is a problem that used to show itself when high speed machining started to take off. there were lots of articles describing the problem and the work around for it.

    Any thoughts? :?
     
  2. Anonymous

    Anonymous New Member

    Offline
    Messages:
    1,280
    Trophy Points:
    0
    If I were home, I'd find it in a second.
    On the Configurations screen, there is a setting for "constant velocity" or something similar. You need to turn it off, to allow each axis' speed to be controlled independently.
    Somebody here will have a machine with Mach installed, who can look it up and give you proper directions.
    Here is a PDF about the settings - http://www.machsupport.com/docs/Mach3_CVSettings_v2.pdf

    You may be interested that there is also a Forum at Artsoft, the folks who write Mach. It's at http://www.machsupport.com/forum/index.php
     
  3. cncmachineguy

    cncmachineguy Member

    Offline
    Messages:
    133
    Trophy Points:
    16
    Location:
    Odenton MD
    Im using EMC2
     
  4. tvcasualty

    tvcasualty New Member

    Offline
    Messages:
    637
    Trophy Points:
    0
    Odd I know of no such option in EMC, I never had this issue at all w/ my MKI. What version of EMC are you running?

    If Tim (gasmasher) does not get on here, shoot him a PM, maybe he will be able to help out as well, I think he uses ECM also.
     
  5. 3DMON

    3DMON Moderator Staff Member

    Offline
    Messages:
    2,380
    Trophy Points:
    38
    Location:
    Sebastian, Florida
    You might want to try exact stop.

    You can put a G61 command before the code starts. This will make the gantry come to a complete stop before it goes around a corner.
     
  6. Anonymous

    Anonymous New Member

    Offline
    Messages:
    1,280
    Trophy Points:
    0
    EMC2?? Oops, sorry. :oops:
     
  7. cncmachineguy

    cncmachineguy Member

    Offline
    Messages:
    133
    Trophy Points:
    16
    Location:
    Odenton MD
    no problem dennis, prolly just empty phlat cup ;)

    Thank you shaun for the g61 tip, I saw that in the phlatscript wish list also, I will try that out!

    funny after 12 years of hand programing machines, never once have I used a g61 - or even knew what it was! Just more proof theres so much to learn about everything and so little time.
     
  8. gasmasher

    gasmasher New Member

    Offline
    Messages:
    402
    Trophy Points:
    0
    Location:
    Atlanta, GA
    Shaun is correct on the G61 except it is called exact path mode. G61.1 is exact stop but I am not sure exactly what the difference is between the two. Just put G61 somewhere near the top after the comments inserted by the PS. It can be on it's own line or add it to the unit setting line (the one with G90 G20 G49).

    You can also try the P parameter to G64. G64 is the fastest route possible no matter how inaccurate. Adding the P parameter lets you specify a maximum distance from the programmed path you are willing to deviate. If you don't like the constant stop/start of G61 you might be able to find a happy medium with G64 P <number>.

    It isn't a clean cut, but my MKII can run through FFF at 600ipm. In G64 mode at those speeds a 3x3" square starts looking a lot like a circle.
     
  9. gasmasher

    gasmasher New Member

    Offline
    Messages:
    402
    Trophy Points:
    0
    Location:
    Atlanta, GA
    I forgot to mention that G61 setting is a feature that can be set in the next version of the PS.
     
  10. cncmachineguy

    cncmachineguy Member

    Offline
    Messages:
    133
    Trophy Points:
    16
    Location:
    Odenton MD
    Thanks tim,

    g61 sounds just like what I am used to. My VMC's get a kinda bump sound when trying to cut above 150ipm on right angles. of course they are a bit heavier. When I first heard it, it used to throw me off for a minuite. Now its just regular.

    being the g61 is modal, I may be able to just MDI it, then be good till a reboot occurs. Sounds like something to play with.

    And yes, just for fun I will have to try 600 ipm at least once!
     

Share This Page