Stop/Start, Jerky, Shutter Movement with Mach3


Results 1 to 14 of 14

Thread: Stop/Start, Jerky, Shutter Movement with Mach3

  1. #1
    Member
    Join Date
    Jul 2012
    Location
    United States
    Posts
    62
    Downloads
    0
    Uploads
    0

    Default Stop/Start, Jerky, Shutter Movement with Mach3

    The Problem
    My CNC machine is stopping & starting between points in G-code on curves. This is making my machine shutter. I noticed it while cutting out of MDF a 30” tall letter “P” for my grandson’s bedroom (Paxton is his name). The g-code has a lot of little short straight runs to create a curve in the letter “P”. I notices a small jumping movement (or shutter, or stop/start movement) at every point, and there are a lot of points. So here is what I found out by reading other posts.

    G64
    First, my g-code has G64 which is for “constant velocity mode”. See line N100 in G-code below.
    N100 G17 G20 G90 G40 G80 G64 G49 G0 M05

    Mach3
    Second, my Mach3 settings that I thought might be important are shown below:

    • “LookAhead” is set to 20 lines.
    • Motion Mode is set to “Constant Velocity”.
    • CV Feedrate is turned off (on the setting page of Mach3).
    • All motors are set the same to 200 ipm, with acceleration set to a low 4 in/sec/sec.
    • Nearly all my cutting is at 30 ipm feed rate, so running too fast, or too high an acceleration rate, is not the problem.

    Computer
    The computer used to run Mach3 is dedicated to just the CNC machine. It is not connected to the internet, no anti-virus, no other program running. Only Mach3 software is loaded on it.

    Need help
    The quality of the cuts is excellent. The CNC machine is doing what it is told to do. But I would like to get rid of whatever is causing the machine to stop/start at every point. I believe there is something in the Mach3 setup or G-Code that is causing this and I do not know what to look for next.

    Thanks for any suggestions.
    Mike

    Similar Threads:


  2. #2
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default

    Turn off CV Distance on the Settings page.
    Increase lookahead to 200.

    In General Config, try turning off all other CV options.

    Have you tried running faster? Or increasing the accel?

    Generally, the faster the accel, the better the performance will be.

    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)


  3. #3
    Member
    Join Date
    Jul 2012
    Location
    United States
    Posts
    62
    Downloads
    0
    Uploads
    0

    Default

    UPDATE: After running several test of different configurations in Mach3, I found out that no matter the Motion Mode is being reset to "Exact Stop" when I start the G-code program, even though I had Motion Mode set to “Constant Velocity” just before running the G-code program. Do not know what is causing this, but believe I am on to something. Any help would be appreciated.

    Again, THANKS,
    Mike



  4. #4
    Member
    Join Date
    Jul 2012
    Location
    United States
    Posts
    62
    Downloads
    0
    Uploads
    0

    Default

    Thanks Gary (ger21) for replying. I did all that you suggested, but no luck. I do think I might had found the problem, but do not know how to fix it. Even though I have the Motion Mode set to “Constant Velocity”, the setting keeps getting changed to “Exact Stop”. I do not know why.

    Nevertheless, do you have any other ideas? Or an idea to why the Motion Mode keeps changing on its own?

    Thanks,
    Mike



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

    Default

    Can you post the g-code?
    When is it being reset, when you load the g-code?

    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
    Jul 2012
    Location
    United States
    Posts
    62
    Downloads
    0
    Uploads
    0

    Default

    Hello Gary,

    This morning, I followed your suggestion in trying to find when the Motion Mode setting is changed from “Constant Velocity” to “Exact Stop”. It does not occur when the program is loaded. It occurs when the program is run. I placed a program stop "M30" after each line (one at a time) and found the the second line in the code "N102 G8 P1" is causing the Motion Mode to change. So I looked up on cnczone.com to find out what that means, and found this posting below:

    If this is for a fanuc, then:
    G08 P1 = Look ahead control ON
    G08 P0 = Look ahead control OFF

    So, I commented out the line, and the Motion Mode setting did NOT changed, it stayed the same at "Constant Velocity" when the program was run again. However, the bad news is it CNC machine still stops/starts at each line segment or point. Guess that was not the problem as I thought it might be, but perhaps combined with something else, it might be part of the problem, or it might not.

    In any case, attached is the code that I been using to test this problem.

    Again, thanks for helping me. I really appreciate you looking at this.
    Mike

    P.S. -- I can not figure out how to attach a file to this reply. Can attach a file when originally writing a post, but not with a reply. Oh well, I have lots to learn. So the code is listed below.

    ======================
    %
    O0000(PAXTON - P-S1)
    (DATE=DD-MM-YY - 04-03-14 TIME=HH:MM - 06:00)
    (MCX FILE - C:\USERS\MIKE\DOCUMENTS\PAXTON P\PAXTON - P - SHEET 1.MCX-6)
    (NC FILE - C:\USERS\MIKE\DOCUMENTS\PAXTON P\PAXTON - P-S1.NC)
    (MATERIAL - WOOD INCH)
    ( T1 | 1/4 STRAIGHT BIT | H1 )

    N100 G17 G20 G90 G40 G80 G64 G49 G0 M05
    N102 G8 P1
    N104 G90 M05 Z5
    N106 G52 X0. Y0. Z0.
    N108 T1 M6

    ( LITTLE CONTOUR CUTOUT ==== )
    N109 g0 z4
    N722 X15 Y18.1359
    N724 Z.25
    N726 G1 Z-.25 F15.
    N728 M98 P1008
    N726 G1 Z-.50 F15.
    N728 M98 P1008
    N738 G1 G90 Z.25 F15.
    N740 G0 Z4.

    N741 x0 y0
    N742 G90 G49 Z5 M05
    N744 G52 X0. Y0. Z0.
    N746 G8 P0
    N748 G17
    N750 M30



    O1008
    N100 G91
    N102 X-.1798 Y-.0302 F30.
    N104 X-.1677 Y-.0361
    N106 X-.1588 Y-.042
    N108 X-.1503 Y-.0476
    N110 X-.1423 Y-.0531
    N112 X-.1347 Y-.0585
    N114 X-.1276 Y-.0636
    N116 X-.1208 Y-.0687
    N118 X-.1144 Y-.0738
    N120 X-.1084 Y-.0789
    N122 X-.1026 Y-.0842
    N124 X-.0982 Y-.0904
    N126 X-.0212 Y-.0209
    N128 X-.109 Y-.1021
    N130 X-.0943 Y-.0988
    N132 X-.084 Y-.0988
    N134 X-.0742 Y-.0989
    N136 X-.0651 Y-.0991
    N138 X-.0565 Y-.0995
    N140 X-.0483 Y-.1001
    N142 X-.0408 Y-.1018
    N144 X-.0203 Y-.0601
    N146 X-.0174 Y-.0588
    N148 X-.0305 Y-.1242
    N150 X-.0278 Y-.1467
    N152 X-.0247 Y-.1727
    N154 X-.0207 Y-.2013
    N156 X-.0158 Y-.2327
    N158 X-.0101 Y-.2672
    N160 X-.0035 Y-.2958
    N162 Y-7.0556
    N164 X.004 Y-.2567
    N166 X.0115 Y-.2413
    N168 X.0186 Y-.2275
    N170 X.0254 Y-.2142
    N172 X.0316 Y-.2016
    N174 X.0376 Y-.1895
    N176 X.0432 Y-.1782
    N178 X.0484 Y-.1673
    N180 X.0535 Y-.157
    N182 X.0582 Y-.1472
    N184 X.0628 Y-.1382
    N186 X.0586 Y-.1137
    N188 X.0759 Y-.1302
    N190 X.0769 Y-.1167
    N192 X.0775 Y-.1042
    N194 X.0781 Y-.0924
    N196 X.0786 Y-.0816
    N198 X.0791 Y-.0716
    N200 X.0798 Y-.0624
    N202 X.0743 Y-.0499
    N204 X.0956 Y-.0543
    N206 X.1132 Y-.055
    N208 X.1402 Y-.0594
    N210 X.1705 Y-.0634
    N212 X.2045 Y-.0676
    N214 X.2425 Y-.0715
    N216 X.2851 Y-.0757
    N218 X.0282 Y-.007
    N220 G2 X.0945 Y-.1213 I-.0305 J-.1213
    N222 G1 Y-2.3437
    N224 G2 X-.1258 Y-.125 I-.125 J0.
    N226 G1 X-.5778 Y.004
    N228 X-.5504 Y.0118
    N230 X-.5229 Y.0191
    N232 X-.4966 Y.0262
    N234 X-.4713 Y.0328
    N236 X-.4467 Y.0391
    N238 X-.4233 Y.045
    N240 X-.4007 Y.0507
    N242 X-.3789 Y.0559
    N244 X-.3582 Y.061
    N246 X-.3381 Y.0656
    N248 X-.319 Y.0702
    N250 X-.3007 Y.0742
    N252 X-.2832 Y.0783
    N254 X-.2664 Y.0819
    N256 X-.2495 Y.0851
    N258 X-.0398 Y.0144
    N260 X-.2806 Y.1106
    N262 X-.2725 Y.116
    N264 X-.2646 Y.1215
    N266 X-.257 Y.1269
    N268 X-.2495 Y.1322
    N270 X-.2423 Y.1375
    N272 X-.2351 Y.1427
    N274 X-.2283 Y.1481
    N276 X-.2215 Y.1533
    N278 X-.2148 Y.1586
    N280 X-.2084 Y.1639
    N282 X-.2021 Y.1692
    N284 X-.1958 Y.1746
    N286 X-.1897 Y.18
    N288 X-.1837 Y.1855
    N290 X-.1778 Y.191
    N292 X-.1719 Y.1968
    N294 X-.1662 Y.2024
    N296 X-.1603 Y.2081
    N298 X-.1292 Y.1778
    N300 X-.1351 Y.2041
    N302 X-.1288 Y.209
    N304 X-.1226 Y.2147
    N306 X-.1166 Y.2205
    N308 X-.1105 Y.2264
    N310 X-.1044 Y.2326
    N312 X-.0983 Y.2388
    N314 X-.0922 Y.2454
    N316 X-.086 Y.2519
    N318 X-.0797 Y.2588
    N320 X-.0734 Y.2659
    N322 X-.067 Y.2731
    N324 X-.0604 Y.2807
    N326 X-.0538 Y.2883
    N328 X-.047 Y.2963
    N330 X-.04 Y.3044
    N332 X-.033 Y.3129
    N334 X-.0258 Y.3216
    N336 X-.0183 Y.3304
    N338 X-.0108 Y.3396
    N340 X-.0029 Y.303
    N342 X.004 Y.3142
    N344 X.012 Y.3072
    N346 X.0198 Y.3003
    N348 X.0274 Y.2935
    N350 X.035 Y.2869
    N352 X.0423 Y.2806
    N354 X.0495 Y.2744
    N356 X.0567 Y.2685
    N358 X.0637 Y.2626
    N360 X.0707 Y.257
    N362 X.0776 Y.2515
    N364 X.0844 Y.2463
    N366 X.0913 Y.2411
    N368 X.098 Y.2361
    N370 X.1049 Y.2313
    N372 X.1116 Y.2265
    N374 X.1184 Y.222
    N376 X.1252 Y.2175
    N378 X.1321 Y.2132
    N380 X.1387 Y.2083
    N382 X.0442 Y.0635
    N384 X.1541 Y.2116
    N386 X.16 Y.2058
    N388 X.1656 Y.1998
    N390 X.1713 Y.1939
    N392 X.1769 Y.1881
    N394 X.1827 Y.1823
    N396 X.1886 Y.1767
    N398 X.1944 Y.1712
    N400 X.2006 Y.1656
    N402 X.2067 Y.1601
    N404 X.2129 Y.1548
    N406 X.2194 Y.1493
    N408 X.2259 Y.144
    N410 X.2326 Y.1386
    N412 X.2395 Y.1333
    N414 X.2465 Y.1279
    N416 X.2538 Y.1224
    N418 X.2611 Y.117
    N420 X.2681 Y.1112
    N422 X.028 Y.0112
    N424 X.2161 Y.0826
    N426 X.2331 Y.0803
    N428 X.2498 Y.0774
    N430 X.2673 Y.0742
    N432 X.2856 Y.0708
    N434 X.305 Y.0673
    N436 X.3253 Y.0633
    N438 X.3465 Y.0592
    N440 X.3688 Y.0548
    N442 X.392 Y.0499
    N444 X.4163 Y.0449
    N446 X.4418 Y.0395
    N448 X.4683 Y.0336
    N450 X.4959 Y.0276
    N452 X.5246 Y.021
    N454 X.5546 Y.0141
    N456 X.5856 Y.0068
    N458 X.2352 Y.0006
    N460 G2 X.1253 Y-.125 I.0003 J-.125
    N462 G1 Y-2.3698
    N464 G2 X-.1042 Y-.1233 I-.125 J0.
    N466 M99
    %

    Last edited by mikefalkner; 03-05-2014 at 08:23 AM. Reason: posted wrong code. Code now correct.


  7. #7
    Member JEST's Avatar
    Join Date
    Nov 2006
    Location
    United States
    Posts
    227
    Downloads
    0
    Uploads
    0

    Default

    Machine would run MUCH smoother with out the polyline code. The "jerks" are directly related to the arcs being converted to polyline segments instead of arcs.



  8. #8
    Member
    Join Date
    Jul 2012
    Location
    United States
    Posts
    62
    Downloads
    0
    Uploads
    0

    Default

    BETTER UNDERSTANDING ??
    Is “Constant Velocity” just for arc or angular movements? And not for the intersection of two straight lines?

    CLUES
    I think I might have hit on the solution – or better understanding – about “Constant Velocity”. Jest’s reply got me thinking. In my research, I found an article at “machsupport.com/wp-content/uploads/2013/02/Mach3_CVSettings_v2.pdf”. This article stated that Constant Velocity mode attempts to maintain a constant velocity during ALL angular or arc moves while obeying the acceleration parameter.” The key words for me were “ALL angular or arc moves”. It appears that “Constant Velocity” does not apply to the connection of two straight lines, as in my case with all the polyline segments instead of arcs. The unfortunate issue for me is that I am using Mastercam and it generated polylines when the arc is not a perfect arc, as is the case with my big letter “P” (see original posting for the reference to the letter “P”).

    TEST
    I tested this by running the simple test code below. Sure enough, the G61 “EXACT STOP” mode will stop/start at the quadrants in the first circle. Reran the same circle (just repositions on x-axis) but with G64 “Constant Velocity”, and it worked!

    CONCLUSION
    So, apparently G64 “Constant Velocity” works for ONLY arc or angular movements, but not with polyline segments as in my code in previous posting.

    QUESTION:
    Is there any code or setting that will provide the “Constant Velocity” effect between polyline segments as with arcs?

    Thanks,
    Mike

    ==== Test Code ====
    %
    N002 (youtube.com/watch?v=FjtamI-LGBk)

    N090 F200 G90 G90.1 (SETUP LINE)

    N100 G61 (EXACT STOP MODE)
    N110 G0 X0 Y0 (BACK TO ZERO)
    N120 G2 X5 Y5 I5 J0 (90 DEG)
    N130 G2 X10 Y0 I5 J0 (90 DEG)
    N140 G2 X5 Y-5 I5 J0 (90 DEG)
    N150 G2 X0 Y0 I5 J0 (90 DEG)

    N180 G0 X10 Y0 (REPOSITION)
    N190 G64 (CV-MODE ON)
    N200 G2 X15 Y5 I15 J0 (90 DEG)
    N210 G2 X20 Y0 I15 J0 (90 DEG)
    N220 G2 X15 Y-5 I15 J0 (90 DEG)
    N230 G2 X10 Y0 I15 J0 (90 DEG)


    N240 G0 X0 Y0 (BACK TO ZERO)
    N260 M30
    %



  9. #9
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default

    CONCLUSION
    So, apparently G64 “Constant Velocity” works for ONLY arc or angular movements, but not with polyline segments as in my code in previous posting.
    That is incorrect. CV mode will indeed "blend" straight segments together to create smoother motion. In G64 mode, your machine should not be stopping at each segment.

    I though that I had replied last night, but it's not here, so maybe I didn't send it?

    Have you tried what I said before?
    Lookahead 200
    CV on (G64)
    All CV settings OFF

    I wonder if the Incremental code (G91) may have something to do with this? Can you get MC to post in Absolute (G90) mode?

    Also, acceleration plays a big part in CV performance, with higher being better. 4 is very low. Can you crank it up a bit?

    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)


  10. #10
    Member
    Join Date
    Jul 2012
    Location
    United States
    Posts
    62
    Downloads
    0
    Uploads
    0

    Default

    Hi Gary,

    I was so happy to had heard from you. I FOUND THE PROBLEM!!! So here is a recap of the problem, test, solution, and conclusion.

    THE PROBLEM
    My CNC machine was stopping and starting at every point with straight segments, and not “blend” together to create a smooth motion when running a G-Code program generated by Mastercam. This occurred regardless of the fact that the Motion Mode setting was “Constant Velocity” and “G64” was included in the code.

    MY TEST METHOD
    Started from scratch and wrote the attached code to test:
    CONSTANT VELOCITY vs EXACT STOP
    ABSOLUTE vs INCREMENTAL
    IJ ARC vs POLYLINE ARC.
    And sure enough, everything worked exactly like Gary told me it would.

    So, went back to my original program that displayed the original problem, and started stripping out code line by line. And in doing so, finally found the solution (after hours of examination, trial and error, ha).

    SOLUTION
    The issue was that my original code generated by Mastercam failed to insert a “G1” code at the beginning of the subroutine that contained all the polyline arcs (see below).

    Note that G1 code is missing in the code below, thus CONSTANT VELOCITY does NOT work.
    O1008
    N100 G91
    N102 X-.1798 Y-.0302 F30.
    N104 X-.1677 Y-.0361
    N106 X-.1588 Y-.042

    N466 M99

    By inserting the code G1 in line N100, the CONSTANT VELOCITY works.
    O1008
    N100 G91 G1
    N102 X-.1798 Y-.0302 F30.
    N104 X-.1677 Y-.0361
    N106 X-.1588 Y-.042

    N466 M99

    CONCLUSION
    In summary, the problem was not related to LookAhead, Motor Acceleration, Absolute vs Increment. You do need Motion Mode set to CV (G64), and in my case, all other CV setting off. And I have increased my LookAhead to 200. The problem was related to a missing G1 in front of all the Polylines. You would had thought my "Post" program would had taken care of this. But it didn't.

    So, G64 works with IJ (arcs) and Polylines (straight lines) provided G1 is included ahead of the Polylines. Now, I have to figure out where in my “Post” program to modify so that G1 is inserted correctly. But at least I now know what the issue was.

    Thanks Gary for helping me.

    ============
    %
    ( ************************************************** ****************** )
    ( * THIS IS A PROGRAM TO TEST EFFECT OF * )
    ( * "CONSTANT VELOCITY" VS "EXACT STOP MODE" * )
    ( * FOR IJ ARCS -- FIRST TWO CIRCLES * )
    ( * FOR POLYLINE ARCS IN ABSOLUTE MODE -- SECOND TWO CIRCLES * )
    ( * FOR POLYLINE ARCS IN INCREMENTAL MODE -- SECOND TWO CIRCLES * )
    ( * * )
    ( * MACH3 SETTINGS: * )
    ( * MOTION MODE = CONSTANT VELOCITY, ALTHOUGH RESET IN CODE BELOW * )
    ( * OTHER CV CONTROLS = UNCHECKED * )
    ( * LOOKAHEAD = 200 * )
    ( * MOTOR ACCELERATION = 4, AND REPEATED AT 20 * )
    ( ************************************************** ****************** )


    ( *************************** )
    ( * TEST WITH IJ ARCS * )
    ( * USING ABSOLUTE G90 MODE * )
    ( *************************** )

    N100 F200 G90 G90.1 (SETUP LINE, USING NON-CUTTING FEEDRATE, & ABSOLUTE MODES)

    N110 G0 X0 Y0 (REPOSITION)
    N120 G64 (CV-MODE ON)
    N130 G2 X5 Y5 I5 J0 (90 DEG)
    N140 G2 X10 Y0 I5 J0 (90 DEG)
    N150 G2 X5 Y-5 I5 J0 (90 DEG)
    N160 G2 X0 Y0 I5 J0 (90 DEG)

    N170 G0 X0 Y0 (REPOSITION)
    N180 G61 (EXACT STOP MODE)
    N190 G2 X5 Y5 I5 J0 (90 DEG)
    N200 G2 X10 Y0 I5 J0 (90 DEG)
    N210 G2 X5 Y-5 I5 J0 (90 DEG)
    N220 G2 X0 Y0 I5 J0 (90 DEG)

    ( *************************** )
    ( * TEST WITH POLYLINE ARCS * )
    ( * USING ABSOLUTE G90 MODE * )
    ( *************************** )

    N225 F200 G90 G90.1 (SETUP LINE, USING NON-CUTTING FEEDRATE, & ABSOLUTE MODES)

    N230 G0 X0 Y0 (REPOSITION)
    N240 G64 (CV-MODE ON)
    N250 M98 P1001 (1ST POLYLINE, ABSOLUTE MODE, CONSTANT VELOCITY MODE)

    N260 G0 G54 X0 Y0 (REPOSITION)
    N270 G61 (EXACT STOP MODE)
    N280 M98 P1001 (2ND POLYLINE, ABSOLUTE MODE, EXACT STOP MODE)

    ( ****************************** )
    ( * TEST WITH POLYLINE ARCS * )
    ( * USING INCREMENTAL G91 MODE * )
    ( ****************************** )


    N285 F200 G90 (SETUP LINE, USING NON-CUTTING FEEDRATE, & ABSOLUTE MODES)

    N290 G0 X0 Y0 (REPOSITION)
    N300 G64 (CV-MODE ON)
    N310 M98 P1002 (3RD POLYLINE SUB, INCREMENTAL MODE, CONSTANT VELOCITY MODE)
    N320 G90 (BACK TO ABSOLUTE MODE)

    N330 G0 G54 X0 Y0 (REPOSITION)
    N340 G61 (EXACT STOP MODE)
    N350 M98 P1002 (4TH POLYLINE SUB, INCREMENTAL MODE, EXACT STOP MODE)
    N360 G90 (BACK TO ABSOLUTE MODE)

    ( *************** )
    ( * END OF TEST * )
    ( *************** )
    N370 G64 (RESET MOTION MODE TO CV)
    N380 G0 X0 Y0 (RETURN TO ZERO)
    N390 M30 (END PROGRAM)


    O1001 (SUB FOR 1ST POLYLINES, 24 LINE CIRCLE, ABSOLUTE MODE)
    N100 G1 X.1704 Y1.2941
    N102 X.6699 Y2.5
    N104 X1.4645 Y3.5355
    N106 X2.5 Y4.3301
    N108 X3.7059 Y4.8296
    N110 X5. Y5.
    N112 X6.2941 Y4.8296
    N114 X7.5 Y4.3301
    N116 X8.5355 Y3.5355
    N118 X9.3301 Y2.5
    N120 X9.8296 Y1.2941
    N122 X10. Y0.
    N124 X9.8296 Y-1.2941
    N126 X9.3301 Y-2.5
    N128 X8.5355 Y-3.5355
    N130 X7.5 Y-4.3301
    N132 X6.2941 Y-4.8296
    N134 X5. Y-5.
    N136 X3.7059 Y-4.8296
    N138 X2.5 Y-4.3301
    N140 X1.4645 Y-3.5355
    N142 X.6699 Y-2.5
    N144 X.1704 Y-1.2941
    N146 X0. Y0.
    N148 M99

    O1002 (SUB FOR 2ND POLYLINES, 24 LINE CIRCLE, INCREMENTAL MODE)
    N100 G91
    N102 G1 X.1704 Y1.2941
    N104 X.4995 Y1.2059
    N106 X.7946 Y1.0355
    N108 X1.0355 Y.7946
    N110 X1.2059 Y.4995
    N112 X1.2941 Y.1704
    N114 X1.2941 Y-.1704
    N116 X1.2059 Y-.4995
    N118 X1.0355 Y-.7946
    N120 X.7946 Y-1.0355
    N122 X.4995 Y-1.2059
    N124 X.1704 Y-1.2941
    N126 X-.1704 Y-1.2941
    N128 X-.4995 Y-1.2059
    N130 X-.7946 Y-1.0355
    N132 X-1.0355 Y-.7946
    N134 X-1.2059 Y-.4995
    N136 X-1.2941 Y-.1704
    N138 X-1.2941 Y.1704
    N140 X-1.2059 Y.4995
    N142 X-1.0355 Y.7946
    N144 X-.7946 Y1.0355
    N146 X-.4995 Y1.2059
    N148 X-.1704 Y1.2941
    N148 M99

    %




  11. #11
    Member
    Join Date
    Jul 2012
    Location
    United States
    Posts
    62
    Downloads
    0
    Uploads
    0

    Default

    UPDATE:
    My Mastercam works perfectly. It inserts G1 in the beginning of the subroutine, the missing of which causes me to start this posting. So, either it was my mistake and I somehow deleted the G1 code in the subroutine, or it was a one-time computer error. I would like to believe it was the computer -- that would make me feel better anyway, ha. But most likely I somehow caused this problem. In any case, problem found and solved.

    Thanks for helping me.
    Mike



  12. #12
    Member
    Join Date
    Jul 2012
    Location
    United States
    Posts
    62
    Downloads
    0
    Uploads
    0

    Default

    SOLVED:
    I was experience “stop and start” action on my CNC machine when there are many short lines that make up a curve that is not a perfectly round arc. The problem deals with the code G64, which is for “Continuous Motion”. Even though G64 was in my G-code and I had all the correct setting in Mach3 (see previous replies to this post), I was still experiencing jerky CNC movement as if the machine was running G61 “Exact Stop”. I finally found the problem after many trial and errors.

    I am using Mastercam to generate G-code for my Mach3 software. In Mastercam, I am using the fanuc generic post. This post outputs a line of g-code that contains G8 P1 at the beginning of the program, and at the end of the program G8 P0. Here is what these code mean:

    G08 P1 = Look ahead control ON
    G08 P0 = Look ahead control OFF

    The G8 code followed the G64 code. For trial and error, I found that the G8 code was canceling the G64 code. Hence, I was running in “Exact Stop” mode.

    To fix this problem, I modified my post. In my post, I found the following line which adds the G8 code:

    if use_g8, pbld, n$, "G8", "P1", e$

    Immediately after that line, I added the following new line:

    pbld, n$, "G64", e$

    Hey, it works! I guess I could had simply commented out the G8 line in the post, but I was not sure what it does for me, so I simply added the new G64 right after it. Like I said, “Hey, it works!”

    Hope this helps someone else.



  13. #13
    Activation process Shawn_M's Avatar
    Join Date
    Oct 2018
    Posts
    29
    Downloads
    0
    Uploads
    0

    Default Re: Stop/Start, Jerky, Shutter Movement with Mach3

    I have a modified HY-6040 machine running with new stepper motors and a G540 with Mach3 and Cut 2D software. My cuts are also excellent but for the life of me I cannot figure out why I also have a lot of little short straight runs to create a curve in my part. I also notice a small jumping movement (or shutter, or stop/start movement) at every point along the part BUT there are very few points. I have read this entire topic and nothing seemed to work. Main difference is I am importing a DXF from AutoCAD. I first join all vectors and then fit curves to vectors. I end up with very few nodes which I thought would be best. I tried the G64 command, all the various CV settings, faster/slower settings and I'm at my wits end. It cuts great but why all the jerking?

    My Mach3 setup is as follows:
    • “LookAhead” is set to 200 lines.
    • Motion Mode is set to “Constant Velocity”.
    • CV Feedrate is turned off (on the setting page of Mach3) and all other CV setting on config are not checked.
    • All motors are set the same to 135 ipm, with acceleration set to 10
    • Nearly all my cutting is at 80 ipm feed rate and I've tried to speed up and slow down with no help

    Computer
    The computer used to run Mach3 is dedicated to just the CNC machine. It is not connected to the internet, no anti-virus, no other program running. Only Mach3 software is loaded on it. 25K kernel speed

    I have tried so many different settings, turning this off and that on and no improvement whatsoever.

    I'm not sure if the post processor is the issue or not. Here's the G code that my Vectric Cut 2D software spits out:

    ( test cut)
    ( File created: Monday April 15 2019 - 04:34 PM)
    ( for Mach2/3 from Vectric )
    ( Material Size)
    ( X= 7.000, Y= 1.750, Z= 0.125)
    ()
    (Toolpaths used in this file)
    (Profile 1)
    (Tools used in this file: )
    (5 = End Mill {0.25 inch})
    N100G00G20G17G90G40G49G80
    N110G70G91.1
    N120T5M06
    N130 (End Mill {0.25 inch})
    N140G00G43Z2.5000H5
    N150S12000M03
    N160(Toolpath:- Profile 1)
    N170()
    N180G94
    N190X0.0000Y0.0000F100.0
    N200G00X-0.1377Y-0.6030Z0.2500
    N210G00Z0.1250
    N220G1Z-0.1260F30.0
    N230G3X1.2097Y-0.4494I-5.5205J54.4290F100.0
    N240G1X1.4700Y-0.4155
    N250G1X1.5904Y-0.3984
    N260G1X1.5924Y-0.3981
    N270G1X3.1625Y-0.1360
    N280G3X3.2183Y-0.1117I-0.0206J0.1233
    N290G3X3.2746Y0.0028I-0.0883J0.1145
    N300G3X3.2179Y0.1175I-0.1444J0.0000
    N310G3X3.1625Y0.1415I-0.0760J-0.0993
    N320G1X1.5924Y0.4036
    N330G1X1.5907Y0.4039
    N340G3X0.6490Y0.5276I-3.3852J-22.1223
    N350G3X-0.4462Y0.6276I-3.2813J-29.8737
    N360G1X-0.6424Y0.6401
    N370G1X-0.7188Y0.6423
    N380G1X-0.7513Y0.6446
    N390G3X-0.8762Y0.6232I-0.0292J-0.2042
    N400G3X-0.9675Y0.5327I0.1014J-0.1936
    N410G1X-2.9205Y0.3918
    N420G1X-2.9345Y0.3900
    N430G3X-3.2550Y0.1121I0.0771J-0.4128
    N440G3X-3.1489Y-0.2838I0.3495J-0.1185
    N450G3X-3.0506Y-0.3478I0.2707J0.3086
    N460G3X-2.9334Y-0.3847I0.2010J0.4343
    N470G1X-2.9205Y-0.3863
    N480G1X-0.9638Y-0.5275
    N490G1X-0.9543Y-0.5368
    N500G3X-0.8372Y-0.6327I0.1858J0.1072
    N510G3X-0.7132Y-0.6438I0.0849J0.2506
    N520G1X-0.6618Y-0.6390
    N530G3X-0.1377Y-0.6030I-0.2933J8.0947
    N540G00Z0.2500
    N550G00Z2.5000
    N560G00X0.0000Y0.0000
    N570M09
    N580M30
    %

    Any help would be great,
    Shawn



  14. #14
    Activation process Shawn_M's Avatar
    Join Date
    Oct 2018
    Posts
    29
    Downloads
    0
    Uploads
    0

    Default Re: Stop/Start, Jerky, Shutter Movement with Mach3

    Well Google saved the day for me. After an exhaustive search and lots of reading I found a post where someone mentioned turning off "CV Feed Rate" in the setting page off, this did the trick.



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

Stop/Start, Jerky, Shutter Movement with Mach3

Stop/Start, Jerky, Shutter Movement with Mach3