Page 2 of 3 FirstFirst 123 LastLast
  1. #11
    Quote Originally Posted by Ger21 View Post
    You must have modified the circle in some way.

    If I export g-code for your circle, it uses G1 segment.
    If I draw a new circle over the top of your, and export g-code, I get G2/G3 moves.

    Nope, just drew it, chose profile and "on-line" offset then output the code.

  2. #12
    Try drawing another circle and doing the same.
    As I said, in your file, if I draw another circle it works, but your circle doesn't.
    Gerry
    ______________________________________________
    UCCNC 2017 Screenset

    Mach3 2010 Screenset

    JointCAM - CAM for Woodworking Joints

  3. #13
    Still messing with this.

    Just imported the same file - a single 19mm circle, drawn in my CAD program, into SheetCam and Aspire. Used the same tool, same profile type, single pass cut, outside edge.

    Sheet cam seems to make the hole in one go...
    N0110 S24000 M03
    N0120 G00 X9.5000 Y-1.0000
    N0130 Z1.0000
    N0140 G01 Z0.000 F250.0
    N0150 G02 X17.2584 Y2.4249 Z-3.0000 I0.0000 J10.5000
    N0160 X17.2584 Y2.4249 I-7.7584 J7.0751 F487.0
    N0170 G00 Z20.0000
    N0180 X0.0000 Y0.0000
    N0190 M09 (Coolant off)
    N0200 M05

    And Aspire seems to do a circle in four arcs?...
    N130 S24000 M03
    N140 (Toolpath:- Profile 1)
    N150 ()
    N160 G94
    N170 X0.000 Y0.000 F377.0
    N180 G00 X0.000 Y10.490 Z20.000
    N190 G00 X0.000 Y10.490 Z2.000
    N200 G01 X0.000 Y10.490 Z-5.100 F377.0
    N210 G02 X10.490 Y0.000 I0.000 J-10.490
    N220 G02 X0.000 Y-10.490 I-10.490 J0.000
    N230 G02 X-10.490 Y0.000 I0.000 J10.490
    N240 G02 X0.000 Y10.490 I10.490 J0.000
    N250 G00 X0.000 Y10.490 Z20.000
    N260 G00 Z20.000
    N270 G00 X0.000 Y0.000
    N280 M05

    Any further ideas?

    The posts for aspire all have ARCS in the names, using a non ARC post generates thousands of very short lines for a circle.

  4. #14
    John S's Avatar
    Lives in Nottingham, England, United Kingdom. Last Activity: 6 Hours Ago Has been a member for 9-10 years. Has a total post count of 2,061. Received thanks 140 times, giving thanks to others 45 times. Referred 1 members to the community.
    Does it matter whether it uses one line or 4 quadrants ?

    post processed literally 1,000's of programs thru Vectric with no hickups
    John S -

  5. #15
    I believe that Aspire always does circles as 4 arcs.
    Gerry
    ______________________________________________
    UCCNC 2017 Screenset

    Mach3 2010 Screenset

    JointCAM - CAM for Woodworking Joints

  6. #16
    Slightly different cutting strategies. Aspire plunges vertically, then cuts the circle in 4 arcs. Sheetcam ramps down in one partial arc, then completes the circle at constant depth (I think - haven't decoded all the coordinates). There also appears to be a 0.05 difference in radius. But I wouldn't worry about the 1 arc/4 arcs difference - in practice, Mach3 is going to optimise its cutting strategy based on looking ahead at a group of moves and the machine parameters and I doubt if it cares!

  7. #17
    Doesn't really matter of course, i just like to know whats going on thats all :)

    Sometimes Aspire seems to resort to making curves from many lines and these were visible in the finish, especially if feed rate override was in use.

  8. #18
    Sometimes Aspire seems to resort to making curves from many lines and these were visible in the finish, especially if feed rate override was in use.
    Not sure what you are saying here. If Aspire generated code with arcs then you turned the federate up in Mach3 that could not change it into small lines.

    I think there is a setting in Mach3 CV that can be ticked.
    ..Clive

  9. #19
    I'm guessing a bit here, but one reason for Aspire's 4-arc strategy might be potential problems with motion controllers. I seem to remember a gcode manual mentioning that some motion controllers could get a bit confused by full turns, so breaking it into arcs could be more reliable. If that was true once, it's probably not relevant any more with the motion controllers we use today but maybe it's just a historical thing?

    There's a discussion of a possible reason here, to do with rounding errors in start/stop points in nearly-full circles. I used to use a free CAM package with LinuxCNC and it often threw up errors with these kind of arc calculations in g2/g3 moves. When I moved to vCarve all those problems went away, so maybe there's sense in it!
    Last edited by Neale; 03-08-2016 at 07:23 AM.

  10. The Following User Says Thank You to Neale For This Useful Post:


  11. #20
    Interesting.

    The one time i noticed it, i was doing a dummy run so had the feedrate turned up to max, it was very jerky on curves, thats what made me think.

    I will need to do some more observing but at least i know now its probably just normal :)

Page 2 of 3 FirstFirst 123 LastLast

Similar Threads

  1. Aspire v4.5
    By m.marino in forum Vectric
    Replies: 6
    Last Post: 16-05-2015, 03:44 PM
  2. Replies: 47
    Last Post: 13-02-2014, 10:49 PM
  3. control signals to draw a circle
    By lakmalp in forum Machine Control Software
    Replies: 3
    Last Post: 16-06-2013, 04:52 PM
  4. Cutting out a circle
    By Martin Paul in forum Machine Discussion
    Replies: 2
    Last Post: 18-04-2011, 11:58 PM
  5. Aspire !!!
    By james mcgrew in forum CAD & CAM Software
    Replies: 2
    Last Post: 17-01-2009, 01:16 AM

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •