Aspire - inefficient G-Code with tabs


Results 1 to 9 of 9

Thread: Aspire - inefficient G-Code with tabs

  1. #1
    Member
    Join Date
    Jan 2008
    Location
    Australia
    Posts
    1523
    Downloads
    2
    Uploads
    0

    Default Aspire - inefficient G-Code with tabs

    Hello all,

    A friend has been generating some gcode via aspire for me.
    I had noted that there seemed to be a pause over the area that a tab will be cut deeper down, as the tool moved along a cut.
    I had a look at the GCode and aspire is putting in x or y moves that correspond to the tabs even when there is no z move.

    For example:
    Rectangle cut with 2 tabs along each side on the rectangle (along the X axis)
    Tabs 3mm high, 4mm long
    Using a 6mm bit
    (Unnecessary lines in red)
    Code:
    N470G1X10.125Y10.125Z-9.000F666.0
    N480G1X10.125Y145.875Z-9.000F2000.0
    N490G1X100.696Y145.875Z-9.000
    N500G1X110.446Y145.875Z-9.000
    N510G1X636.093Y145.875Z-9.000
    N520G1X645.843Y145.875Z-9.000
    N530G1X745.875Y145.875Z-9.000
    N540G1X745.875Y10.125Z-9.000
    N550G1X639.981Y10.125Z-9.000
    N560G1X630.231Y10.125Z-9.000
    N570G1X114.354Y10.125Z-9.000
    N580G1X104.604Y10.125Z-9.000
    N590G1X10.125Y10.125Z-9.000
    N600G1X10.125Y10.125Z-12.000F666.0
    N610G1X10.125Y145.875Z-12.000F2000.0
    N620G1X100.696Y145.875Z-12.000
    N630G1X100.696Y145.875Z-9.000
    N640G1X110.446Y145.875Z-9.000
    N650G1X110.446Y145.875Z-12.000F666.0
    N660G1X636.093Y145.875Z-12.000F2000.0
    N670G1X636.093Y145.875Z-9.000
    N680G1X645.843Y145.875Z-9.000
    N690G1X645.843Y145.875Z-12.000F666.0
    N700G1X745.875Y145.875Z-12.000F2000.0
    N710G1X745.875Y10.125Z-12.000
    N720G1X639.981Y10.125Z-12.000
    N730G1X639.981Y10.125Z-9.000
    N740G1X630.231Y10.125Z-9.000
    N750G1X630.231Y10.125Z-12.000F666.0
    N760G1X114.354Y10.125Z-12.000F2000.0
    N770G1X114.354Y10.125Z-9.000
    N780G1X104.604Y10.125Z-9.000
    N790G1X104.604Y10.125Z-12.000F666.0
    N800G1X10.125Y10.125Z-12.000F2000.0
    N810G00X10.125Y10.125Z10.000
    Is there a setting to avoid this? It's unnecessary code, and does seem to cause a slight tool slow down at these points. (Maybe I just need to fiddle with my Mach3 constant velocity settings?)

    Thoughts?

    Similar Threads:


  2. #2
    Registered cutter100's Avatar
    Join Date
    May 2010
    Location
    us
    Posts
    63
    Downloads
    0
    Uploads
    0

    Default

    I think the best bet would be to get in touch with Vectric and see what they say. Although it would kind of suck...you could scan through your code each time and maybe delete the lines?
    I have no idea if there's a work around for this. Just out of curiosity how much time does it waste?

    Chris.....Everyday is a Good day.....if you wake up breathing!
    Joe's 2006, Mach3, Vectric software.


  3. #3
    Registered
    Join Date
    Oct 2004
    Location
    USA
    Posts
    590
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by pippin88 View Post
    Is there a setting to avoid this? It's unnecessary code, and does seem to cause a slight tool slow down at these points. (Maybe I just need to fiddle with my Mach3 constant velocity settings?)

    Thoughts?
    If you break the code into two parts you can eliminate this problem.
    Part 1: Cut down to the level of the tabs.
    Part 2: Cut from the tab level to the bottom of the material.

    I have Vcarve Pro 6.5 and this was easy to do. The only wasted move then was going back to clearance height before running the second part. This point is easily located and can be edited out of the code if necessary. The combined files are attached.

    Chris

    Code:
    ( VectricTest052612 )
    ( File created: Saturday, May 26, 2012 - 08:12 PM)
    ( for Mach2/3 from Vectric )
    ( Material Size)
    ( X= 10.000, Y= 8.000, Z= 0.500)
    ()
    (Toolpaths used in this file:)
    (Test1a)
    (Test1b)
    (Tools used in this file: )
    (1 = End Mill [0.25 inch])
    N110G00G20G17G90G40G49G80
    N120G70G91.1
    N130T1M06
    N140 (End Mill [0.25 inch])
    N150G00G43Z0.8000H1
    N160S12000M03
    N170(Toolpath:- Test1a)
    N180()
    N190G94
    N200X0.0000Y0.0000F100.0
    N210G00X1.8477Y1.9597Z0.2000
    N220G1Z-0.0938F30.0
    N230G2X1.7227Y2.0847I0.0000J0.1250F100.0
    N240G1Y5.9495
    N250G2X1.8477Y6.0745I0.1250J0.0000
    N260G1X7.7077
    N270G2X7.8327Y5.9495I0.0000J-0.1250
    N280G1Y2.0847
    N290G2X7.7077Y1.9597I-0.1250J0.0000
    N300G1X1.8477
    N310G1Z-0.1875F30.0
    N320G2X1.7227Y2.0847I0.0000J0.1250F100.0
    N330G1Y5.9495
    N340G2X1.8477Y6.0745I0.1250J0.0000
    N350G1X7.7077
    N360G2X7.8327Y5.9495I0.0000J-0.1250
    N370G1Y2.0847
    N380G2X7.7077Y1.9597I-0.1250J0.0000
    N390G1X1.8477
    N400G1Z-0.2813F30.0
    N410G2X1.7227Y2.0847I0.0000J0.1250F100.0
    N420G1Y5.9495
    N430G2X1.8477Y6.0745I0.1250J0.0000
    N440G1X7.7077
    N450G2X7.8327Y5.9495I0.0000J-0.1250
    N460G1Y2.0847
    N470G2X7.7077Y1.9597I-0.1250J0.0000
    N480G1X1.8477
    N490G1Z-0.3750F30.0
    N500G2X1.7227Y2.0847I0.0000J0.1250F100.0
    N510G1Y5.9495
    N520G2X1.8477Y6.0745I0.1250J0.0000
    N530G1X7.7077
    N540G2X7.8327Y5.9495I0.0000J-0.1250
    N550G1Y2.0847
    N560G2X7.7077Y1.9597I-0.1250J0.0000
    N570G1X1.8477
    (COMMENT OUT THE LINE BELOW)
    (N580G00Z0.2000)
    N590S12000M03
    (Test1b)
    (COMMENT OUT THE LINE BELOW)
    (N620G00X1.8477Y1.9597Z0.2000)
    N630G1Z-0.5000F30.0
    N640G2X1.7227Y2.0847I0.0000J0.1250F100.0
    N650G1Y5.9495
    N660G2X1.8477Y6.0745I0.1250J0.0000
    N670G1X2.4703
    N680G1Z-0.3750
    N690G1X3.2203
    N700G1Z-0.5000F30.0
    N710G1X6.2104F100.0
    N720G1Z-0.3750
    N730G1X6.9604
    N740G1Z-0.5000F30.0
    N750G1X7.7077F100.0
    N760G2X7.8327Y5.9495I0.0000J-0.1250
    N770G1Y2.0847
    N780G2X7.7077Y1.9597I-0.1250J0.0000
    N790G1X7.0851
    N800G1Z-0.3750
    N810G1X6.3351
    N820G1Z-0.5000F30.0
    N830G1X3.2798F100.0
    N840G1Z-0.3750
    N850G1X2.5298
    N860G1Z-0.5000F30.0
    N870G1X1.8477F100.0
    N880G00Z0.2000
    N890G00Z0.8000
    N900G00X0.0000Y0.0000
    N910M09
    N920M30
    %


    Attached Files Attached Files
    Last edited by OCNC; 05-26-2012 at 08:49 PM.


  4. #4
    Member
    Join Date
    Jan 2008
    Location
    Australia
    Posts
    1523
    Downloads
    2
    Uploads
    0

    Default

    It's easy enough to do manually, or to do two toolpaths. But really that shouldn't have to be done, the toolpath generation should deal with it.
    I might raise it with the Vectric directly.



  5. #5
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default

    Quote Originally Posted by pippin88 View Post
    It's easy enough to do manually, or to do two toolpaths. But really that shouldn't have to be done, the toolpath generation should deal with it.
    I might raise it with the Vectric directly.
    It has to do with the algorithm that Vectric uses to create the toolpaths. From what I've heard, it would require a lot of work to change.

    As you mentioned, try playing with your CV settings to see if you can get Mach3 to ignore them.

    Gerry

    UCCNC 2017 Screenset
    [URL]http://www.thecncwoodworker.com/2017.html[/URL]

    Mach3 2010 Screenset
    [URL]http://www.thecncwoodworker.com/2010.html[/URL]

    JointCAM - CNC Dovetails & Box Joints
    [URL]http://www.g-forcecnc.com/jointcam.html[/URL]

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  6. #6
    Member
    Join Date
    Apr 2007
    Location
    USA
    Posts
    8082
    Downloads
    0
    Uploads
    0

    Default

    I don't know if it will help in this instance, but it may be useful to know that when you create closed vectors you can node edit them and move the start point anywhere you want it to be by clicking on an option to change an existing node (black square dot) to a start point (green square dot) or you can add a new node where you want it to be and define it as the start point.

    I'm thinking that a start point next to a tab can cause some strange looking moves. May be worth investigating.

    CarveOne
    http://www.carveonecncwoodcraft.com


  7. #7
    Registered
    Join Date
    May 2011
    Location
    Canada
    Posts
    3
    Downloads
    0
    Uploads
    0

    Default Re: Aspire - inefficient G-Code with tabs

    Hi,
    Have you ever figured this problem out... I'm having the same issue with Aspire and Mach 3. It's just a slight stutter but it affects my cuts
    Cheers
    Lyle



  8. #8
    Member
    Join Date
    Jan 2008
    Location
    Australia
    Posts
    1523
    Downloads
    2
    Uploads
    0

    Default Re: Aspire - inefficient G-Code with tabs

    I now use LinuxCNC. Aspire 8 I think

    I haven't noticed the issue for a long time. However, I tend to use 3D tabs now, which may be different.



  9. #9
    Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5516
    Downloads
    0
    Uploads
    0

    Default Re: Aspire - inefficient G-Code with tabs

    Check your part too, make sure that section is one straight line, not a cluster of nodes in a straight line... aside from the normal CV settings check the look ahead number, it's default very low like 10 or 20 lines.



Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Aspire - inefficient G-Code with tabs

Aspire - inefficient G-Code with tabs