584,817 active members*
4,973 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Autodesk CAM > Inventor GCODE Post Issue Accumulating Error Circular Interpolation
Results 1 to 3 of 3
  1. #1
    Join Date
    Apr 2019
    Posts
    1

    Inventor GCODE Post Issue Accumulating Error Circular Interpolation

    For those that like GCode and like a simple challenge:....

    I am using Inventor to generate some GCode (Linux Post).
    I am performing some calculations and seem to keep running into a weird accumulating offset on my machine. I have done some manual calculations and I can definitely see there is something that doesn't add up. It seems to be on Circular Interpolation (G17 so X&Y). I have attached the code below.

    My problem is in a facing operation where I perform a series of circular interpolations. The first few go amazingly well, landing exactly on point, however when it comes to line N115 I am out by 1.
    It then seems to keep getting worse from that point.

    Working through line N115, I have a starting point of Y: -52.874 (N105 is the last time YAxis value changed), i then cut a circle with an offset of 1.886 in the same Y-Axis. So theoretically I should land at -58.874 + 1.886 + 1.886 = -49.102 but the GCode states that I should land at -49.101.

    Now I know most of you are going to say rounding, but with this precision there is no rounding.

    How is it that the GCODE calculating -49.101. This means that my next instruction is off by one and keeps accumulating errors as it proceeds.

    It is absolute programming but due to the fact that it is a facing operation with only circular interpolations affecting the Y axis value; it means that there will always be an error cause I have to take either my calculated value or use the calculated value in the GCode. If I use my calculated value then it means I wont match with the next circular interpolation value and if I use the GCode Y value then it wont match with the formula for a circle/arc.

    Even when I use NCViewer to model the GCode I can see that it calculates -49.102; could it be that Inventor just doesn't calculate G codes correctly?


    This simple program starts at :

    I have the following instructions:

    %
    (LINUXGCODE)
    (T5 D=4. CR=0. - ZMIN=-20.49 - FLAT END MILL)
    N10 G90 G94 G17 G91.1
    N15 G21
    N20 G53 G0 Z0.
    (FACE1)
    N25 M9
    N30 T5 M6
    N35 S5000 M3
    N40 G54
    N45 M8
    N50 G0 X68.6 Y-64.19
    N55 G43 Z15. H5
    N60 G0 Z5.
    N65 G1 Z-0.6 F500.
    N70 G18 G3 X68.2 Z-1. I-0.4 K0.
    N75 G1 X66.
    N80 X-66. F1000.
    N85 G17 G2 Y-60.418 I0. J1.886
    N90 G1 X66.
    N95 G3 Y-56.646 I0. J1.886
    N100 G1 X-66.
    N105 G2 Y-52.874 I0. J1.886
    N110 G1 X66.
    N115 G3 Y-49.101 I0. J1.886
    N120 G1 X-66.
    N125 G2 Y-45.329 I0. J1.886
    N130 G1 X66.
    N135 G3 Y-41.557 I0. J1.886
    N140 G1 X-66.
    N145 G2 Y-37.785 I0. J1.886
    N150 G1 X66.

  2. #2
    Join Date
    Jun 2008
    Posts
    1838

    Re: Inventor GCODE Post Issue Accumulating Error Circular Interpolation

    Well, I don`t think that you have anything to really worry about, the error is only 0.001 of a millimeter and is not cumulitive as once that line is the 0.001mm out all the susequent lines still do a 3.772mm step over so at the end there is still only a total of 0.001mm error.
    It is possibly to do with the settings in your program, there will likely be a Tolerance setting that is possibly set too low and allowing the post processor to spit out these tiny differences, I don`t have Inventor so not able to check on the way the settings are done but have a look for the program tolerances and if it is for example to 4 decimals like 0.0001mm then try changing it to a more reasonable 0.01mm and see what you get then

    Yes the code should read in brackets Red :-

    %
    (LINUXGCODE)
    (T5 D=4. CR=0. - ZMIN=-20.49 - FLAT END MILL)
    N10 G90 G94 G17 G91.1
    N15 G21
    N20 G53 G0 Z0.
    (FACE1)
    N25 M9
    N30 T5 M6
    N35 S5000 M3
    N40 G54
    N45 M8
    N50 G0 X68.6 Y-64.19
    N55 G43 Z15. H5
    N60 G0 Z5.
    N65 G1 Z-0.6 F500.
    N70 G18 G3 X68.2 Z-1. I-0.4 K0.
    N75 G1 X66.
    N80 X-66. F1000.
    N85 G17 G2 Y-60.418 I0. J1.886
    N90 G1 X66.
    N95 G3 Y-56.646 I0. J1.886
    N100 G1 X-66.
    N105 G2 Y-52.874 I0. J1.886
    N110 G1 X66.
    N115 G3 Y-49.101 I0. J1.886 (Y-49.102)
    N120 G1 X-66.
    N125 G2 Y-45.329 I0. J1.886 (Y-45.330)
    N130 G1 X66.
    N135 G3 Y-41.557 I0. J1.886 (Y-41.558)
    N140 G1 X-66.
    N145 G2 Y-37.785 I0. J1.886 (Y-37.786)
    N150 G1 X66.

    As I suspect that that amount of 0.001mm is probably less than your machines control resolution and almost certainly less than your machines mechanical resolution which for most machines (Especially if it uses Stepper Motors) is only 0.01mm so those tiny differences will probably never be noticed by your control and will never affect a cut so unless you notice any future larger deviations then just carry on as normal.

    Hope tha is of some help to you

    Regards
    Rob

  3. #3
    Join Date
    Dec 2008
    Posts
    3110

    Re: Inventor GCODE Post Issue Accumulating Error Circular Interpolation

    You not out by 1. you are out by 1 micron (0.001)
    you seem to be doing a facing operation..... does this error in the middle of a cleared area really matter ?
    Is it giving an alarm while machining ?

    It is a rounding error, a 1/2 circle Y move at the end of each X move.... if you really dug down deep... each position is probably calculated to 15 decimal places.. & the NC output is only 3 decimal places for metric, this shows up as the consistent rad size and the discrepancy with X or Y value. I would not be overly concerned with this error unless it stops the machine from running.

Similar Threads

  1. Circular interpolation issue
    By nzben in forum Cincinnati CNC
    Replies: 13
    Last Post: 06-18-2012, 11:10 AM
  2. Axis' don't return to zero - accumulating error
    By Scott Kelley in forum Servo Motors / Drives
    Replies: 23
    Last Post: 05-05-2011, 01:25 PM
  3. G540 .xml / Mach3 / gcode error issue
    By forrest39 in forum Benchtop Machines
    Replies: 3
    Last Post: 06-30-2010, 12:11 AM
  4. circular interpolation
    By pmesilver in forum Mach Mill
    Replies: 1
    Last Post: 04-10-2010, 01:20 PM
  5. Circular Interpolation
    By Deadwood in forum Mach Software (ArtSoft software)
    Replies: 3
    Last Post: 01-11-2009, 09:35 PM

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
  •