Need Help! Problems with Fusion 360 toolpaths


Page 1 of 3 123 LastLast
Results 1 to 20 of 41

Thread: Problems with Fusion 360 toolpaths

  1. #1
    Registered
    Join Date
    Jul 2007
    Location
    Canada
    Posts
    139
    Downloads
    0
    Uploads
    0

    Default Problems with Fusion 360 toolpaths

    I'm trying to troubleshoot some issues with stuttering and jerky moves on my CNC router. I'm using a UCCNC controller and I have been finding that some fusion G code leads to stuttering and chatter marks on my parts. My CNC router uses ballscrews on all axis and linear profile rails, along with leadshine easy servos, and is capable of very smooth motion after tuning the acceleration values in the controller software.
    As far as G code goes, I've tried smoothing values up to .005" and sometimes that helps, but not always. Typically the stuttering is on finish passes too, so between cutting wood with a sharp cutter and light passes there should be no mechanical reason for the chatter. I can sometimes hear and feel the machine rapidly accelerate and decelerate both on complex 3D surfacing and even sometimes on simple 2D paths. My current theory is that Fusion G code is overriding my controllers default acceleration as the servos have more than enough torque to shake the whole machine when their acceleration values are set too high. When the G code has lots of small segments this pulsing could occur. I also occasionally hear a loud thunk when cutting, which might be the cutter hitting a hard spot, but sounds a lot more like the sound of a motor coming to a quick stop.
    For a bit more reference, I can jog the machine @ 600ipm with smooth acceleration and have no noticeable shake, but running a program at anywhere between 100-250 ipm can cause noticeable shake and chatter.
    Can anyone recommend settings to tweak or other possible solutions to this problem.

    Similar Threads:


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

    Default Re: Problems with Fusion 360 toolpaths

    I think that you need to play with the CV settings in UCCNC.
    Linear error, Linear unify, and Linear Addition.

    My current theory is that Fusion G code is overriding my controllers default acceleration
    G-code has no control over acceleration, so this is not possible.

    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
    Registered
    Join Date
    Jul 2007
    Location
    Canada
    Posts
    139
    Downloads
    0
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Quote Originally Posted by ger21 View Post
    I think that you need to play with the CV settings in UCCNC.
    Linear error, Linear unify, and Linear Addition.



    G-code has no control over acceleration, so this is not possible.
    I thought the same thing, but was second guessing it because the acceleration values I set in UCCNC seemed to work well. I will play with these values and see what happens


    Sent from my iPhone using Tapatalk



  4. #4
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Your acceleration settings may be fine. UCCNC will try to follow as close to the path as it can, dictated by the CV settings.If it needs to slow down to follow the path, it will. By loosening up the tolerances a little, it may be able to run smoother.

    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)


  5. #5
    Member
    Join Date
    Jan 2005
    Location
    USA
    Posts
    1943
    Downloads
    2
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Is the G-code running in exact stop mode? Look at the G-code to see if there is a G61 or a G61.1. These are for exact stop, which means that the machine will briefly come to a stop at each programmed point no matter what. G64 is path blending mode and is used to keep the speed up. when the machine goes from move to move the controller has to calculate acceleration and deceleration to keep the path within the CV settings and will try to keep the speed up as much as possible. So lets say you have 2 programmed line moves and there is no angle change between them. In G64, the machine won't have to slow down at all between those moves, but in G61 it will come to a complete stop even though the moves are in the same direction. Likewise a 90 degree turn will result in a tiny bit or rounding in the corner when in G64, but not when in G61.



  6. #6
    Registered
    Join Date
    Jul 2007
    Location
    Canada
    Posts
    139
    Downloads
    0
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    The controller is set to CV, however there is no G61 or G64 anywhere in the code. Not sure if adding a G64 would change anything but I'll test it out


    Sent from my iPhone using Tapatalk



  7. #7
    Registered
    Join Date
    Jul 2007
    Location
    Canada
    Posts
    139
    Downloads
    0
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Quote Originally Posted by ger21 View Post
    Your acceleration settings may be fine. UCCNC will try to follow as close to the path as it can, dictated by the CV settings.If it needs to slow down to follow the path, it will. By loosening up the tolerances a little, it may be able to run smoother.
    I loosened up the cv values and some tool paths run a little smoother while others may have gotten a little worse. I have my servos set up to trigger an emergency stop if they overshoot too far or draw too much current and the z axis triggered for some strange reason. I got some video footage of the stuttering and the thunk the z axis sometimes makes. These problems are still happening with the feed rate turned way down and the cuts are pretty light as well.

    Can't seem to upload the video right now but I'll try again later from a computer


    Sent from my iPhone using Tapatalk



  8. #8
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Can you post the g-code, and some pics of what you're getting?

    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)


  9. #9
    Registered
    Join Date
    Jul 2007
    Location
    Canada
    Posts
    139
    Downloads
    0
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    So I finally got some video footage uploaded, and hopefully that will give you a better reference to see the issues I'm having. I did a dry run with the feed turned way down, and you can hear and see that the speed is ramping up and down with each line of code. I'm scratching my head a bit here as these tool paths are smooth (smoothing set to .005") and there's no sharp angles that should be causing the acceleration to change, so I would think that they would flow at uniform speed. The thunk noises are especially annoying as they seem to be random, can happen on a simple 2D path as well, and happen at random times and positions. I can't completely rule out a mechanical cause, but it's the same thunk sound as when the motors are first energized or if they had to come to a rapid stop, which leads me to believe something electrical or code related is causing it.

    Slow speed test https://goo.gl/photos/t6gLbUsFHd45SKgMA
    High speed test https://goo.gl/photos/PTzbuGX8zV5Wt6zy5
    Thunk during dry run https://goo.gl/photos/W8exqxHgkm27mw6N9
    Cutting wood https://goo.gl/photos/nSusAV2DED7mcvUx5 (listen for thunk 4 seconds in)

    In the UCCNC software I've increased the buffer size to .5, made sure it's in CV mode, changed look ahead lines to 500, linear error and corner error tested in increments from .03 to .5 (larger corner error helps a bit but doesn't eliminate the problem and probably introduces new ones). I'm not sure effect the what the linear addition length and linear unify length have but I tested them from 1 to 10 without any noticeable effect.

    Is there something I'm missing here?


    Here's a section of the G code
    [1001]
    [CNC Router]
    [T3 D=19.05 CR=9.525 - ZMIN=-6.17 - ball end mill]
    G90
    G22
    G53
    [Radial1 (3)]
    T3
    S18000 M3
    M37 H3
    G0 X201.296 Y130.997
    G43 Z116.84
    Z83.319
    G1 Z83.192 F6350
    X201.303 Z83.026
    X201.325 Z82.862
    X201.361 Z82.7
    X201.411 Z82.541
    X201.474 Z82.388
    X201.551 Z82.24
    X201.64 Z82.1
    X201.741 Z81.968
    X201.853 Z81.846
    X201.976 Z81.733
    X202.108 Z81.632
    X202.248 Z81.543
    X202.395 Z81.466
    X202.549 Z81.403
    X202.707 Z81.353
    X202.869 Z81.317
    X203.034 Z81.295
    X203.2 Z81.287
    X285.829 Z81.255
    X286.207 Z81.216
    X286.583 Z81.162
    X286.957 Z81.094
    X287.328 Z81.01
    X287.695 Z80.912
    X288.058 Z80.799
    X288.417 Z80.672
    X288.77 Z80.531
    X289.117 Z80.376
    X289.457 Z80.207
    X289.791 Z80.025
    X290.117 Z79.829
    X290.435 Z79.621
    X290.744 Z79.4
    X291.045 Z79.167
    X291.336 Z78.922
    X291.617 Z78.666
    X291.887 Z78.399
    X292.147 Z78.121
    X292.395 Z77.834
    X292.632 Z77.536
    X292.857 Z77.23
    X293.069 Z76.914
    X293.269 Z76.591
    X293.455 Z76.259
    X293.629 Z75.921
    X293.788 Z75.576
    X293.934 Z75.225
    X294.065 Z74.868
    X294.183 Z74.506
    X294.286 Z74.14
    X294.374 Z73.771
    X294.447 Z73.398
    X294.506 Z73.022
    X294.549 Z72.644
    X294.605 Z72.108
    X294.677 Z71.573
    X294.764 Z71.041
    X294.867 Z70.512
    X294.986 Z69.986
    X295.12 Z69.463
    X295.269 Z68.945
    X295.433 Z68.431
    X295.612 Z67.922
    X295.806 Z67.419
    X296.015 Z66.922
    X296.238 Z66.431
    X296.475 Z65.946
    X296.726 Z65.469
    X296.992 Z65.
    X297.27 Z64.538
    X297.563 Z64.085
    X297.868 Z63.64
    X298.186 Z63.205
    X300.641 Z59.755
    X303.136 Z56.785
    X307.478 Z52.341
    X312.628 Z47.759
    X319.026 Z42.723
    X326.283 Z37.558
    X336.526 Z30.881
    X348.785 Z23.487
    X367.044 Z13.113
    X373.062 Z9.792
    X375.593 Z9.761
    X375.705 Z9.767
    X375.814 Z9.785
    X375.921 Z9.815
    X376.024 Z9.858
    X376.124 Z9.901
    X376.228 Z9.931
    X376.335 Z9.949
    X376.443 Z9.956
    X376.816 Y131.021 Z9.95
    X377.183 Y131.092 Z9.935
    X377.537 Y131.209 Z9.908
    X377.872 Y131.371 Z9.872
    X378.183 Y131.574 Z9.827
    X378.464 Y131.814 Z9.774
    X378.71 Y132.088 Z9.713
    X378.918 Y132.392 Z9.645
    X379.083 Y132.719 Z9.572
    X379.203 Y133.064 Z9.495
    X379.276 Y133.422 Z9.416
    X379.301 Y133.786 Z9.334
    Y134.224 Z9.237
    X379.276 Y134.588 Z9.156
    X379.203 Y134.946 Z9.076
    X379.083 Y135.291 Z8.999
    X378.918 Y135.618 Z8.926
    X378.71 Y135.922 Z8.859
    X378.464 Y136.196 Z8.798
    X378.183 Y136.437 Z8.744
    X377.872 Y136.639 Z8.699
    X377.537 Y136.801 Z8.663
    X377.183 Y136.918 Z8.637
    X376.816 Y136.989 Z8.621
    X376.443 Y137.013 Z8.616
    X375.893
    X375.784 Z8.61
    X375.678 Z8.591
    X375.573 Z8.561
    X375.473 Z8.519
    X375.368 Y137.009 Z8.475
    X375.258 Y137.006 Z8.443
    X375.145 Y137.002 Z8.426
    X375.03 Y136.998 Z8.422
    X372.589 Y136.912 Z8.484
    X362.35 Y136.555 Z14.268
    X346.964 Y136.017 Z23.269
    X335.93 Y135.632 Z30.097
    X326.498 Y135.303 Z36.367
    X318.703 Y135.031 Z42.036
    X312.24 Y134.805 Z47.244
    X307.33 Y134.633 Z51.692
    X303.453 Y134.498 Z55.707
    X300.222 Y134.385 Z59.566
    X299.81 Y134.371 Z60.066
    X299.41 Y134.357 Z60.575
    X299.022 Y134.343 Z61.094
    X298.645 Y134.33 Z61.621
    X298.281 Y134.317 Z62.156
    X297.929 Y134.305 Z62.7
    X297.589 Y134.293 Z63.251
    X297.262 Y134.282 Z63.811
    X296.948 Y134.271 Z64.377
    X296.647 Y134.26 Z64.951
    X296.359 Y134.25 Z65.531
    X296.084 Y134.241 Z66.117
    X295.823 Y134.232 Z66.71
    X295.575 Y134.223 Z67.309
    X295.341 Y134.215 Z67.913
    X295.121 Y134.207 Z68.522
    X294.915 Y134.2 Z69.136
    X294.722 Y134.193 Z69.755
    X294.544 Y134.187 Z70.377
    X294.381 Y134.181 Z71.004
    X294.394 Y134.182 Z71.395
    X294.392 Z71.786




  10. #10
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    I'm not sure effect the what the linear addition length and linear unify length have but I tested them from 1 to 10 without any noticeable effect.
    I believe that thee settings should be much lower, as your g-code consists of lots of straight segments, 0.1mm long.

    Also. do you have backlash comp enabled?

    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)


  11. #11
    Member
    Join Date
    Jun 2015
    Location
    Sweden
    Posts
    943
    Downloads
    0
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Quote Originally Posted by Andrew22 View Post
    So I finally got some video footage uploaded, and hopefully that will give you a better reference to see the issues I'm having. I did a dry run with the feed turned way down, and you can hear and see that the speed is ramping up and down with each line of code. I'm scratching my head a bit here as these tool paths are smooth (smoothing set to .005") and there's no sharp angles that should be causing the acceleration to change, so I would think that they would flow at uniform speed. The thunk noises are especially annoying as they seem to be random, can happen on a simple 2D path as well, and happen at random times and positions. I can't completely rule out a mechanical cause, but it's the same thunk sound as when the motors are first energized or if they had to come to a rapid stop, which leads me to believe something electrical or code related is causing it.

    Slow speed test https://goo.gl/photos/t6gLbUsFHd45SKgMA
    High speed test https://goo.gl/photos/PTzbuGX8zV5Wt6zy5
    Thunk during dry run https://goo.gl/photos/W8exqxHgkm27mw6N9
    Cutting wood https://goo.gl/photos/nSusAV2DED7mcvUx5 (listen for thunk 4 seconds in)

    In the UCCNC software I've increased the buffer size to .5, made sure it's in CV mode, changed look ahead lines to 500, linear error and corner error tested in increments from .03 to .5 (larger corner error helps a bit but doesn't eliminate the problem and probably introduces new ones). I'm not sure effect the what the linear addition length and linear unify length have but I tested them from 1 to 10 without any noticeable effect.

    Is there something I'm missing here?


    Here's a section of the G code
    Try increase the acceleration parameter on your axes to a value which your axes can handle as maximum.
    Try set the unify and additions in the CV larger, ie. values 100 for a test
    Set the linear and corners error according to what tolerances your job will allow.



  12. #12
    Registered
    Join Date
    Feb 2009
    Location
    USA
    Posts
    311
    Downloads
    0
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Quote Originally Posted by Andrew22 View Post
    So I finally got some video footage uploaded, and hopefully that will give you a better reference to see the issues I'm having. I did a dry run with the feed turned way down, and you can hear and see that the speed is ramping up and down with each line of code. I'm scratching my head a bit here as these tool paths are smooth (smoothing set to .005") and there's no sharp angles that should be causing the acceleration to change, so I would think that they would flow at uniform speed. The thunk noises are especially annoying as they seem to be random, can happen on a simple 2D path as well, and happen at random times and positions. I can't completely rule out a mechanical cause, but it's the same thunk sound as when the motors are first energized or if they had to come to a rapid stop, which leads me to believe something electrical or code related is causing it.

    Slow speed test https://goo.gl/photos/t6gLbUsFHd45SKgMA
    High speed test https://goo.gl/photos/PTzbuGX8zV5Wt6zy5
    Thunk during dry run https://goo.gl/photos/W8exqxHgkm27mw6N9
    Cutting wood https://goo.gl/photos/nSusAV2DED7mcvUx5 (listen for thunk 4 seconds in)

    In the UCCNC software I've increased the buffer size to .5, made sure it's in CV mode, changed look ahead lines to 500, linear error and corner error tested in increments from .03 to .5 (larger corner error helps a bit but doesn't eliminate the problem and probably introduces new ones). I'm not sure effect the what the linear addition length and linear unify length have but I tested them from 1 to 10 without any noticeable effect.

    Is there something I'm missing here?


    Here's a section of the G code


    If you have smoothing turned (in Fusion) on then something is not right because that code has no arcs in it. My guess is that your post is ignoring it for some reason. What post are you using? It would also help if you could post the Fusion project so we can see the operation settings. Having lots of tiny line movements can overload the controller's look ahead buffer and cause data starvation. This tends to cause sort of a stutter or chatter in the motion. Other than that the code looks ok.

    I'm thinking the thunk noise is something unrelated to the code, like an intermittent electrical connection, or even something mechanical. This is where you'll have to go around wiggling connectors and banging on things to see if you can induce the problem.


    C|



  13. #13
    Registered
    Join Date
    Jul 2007
    Location
    Canada
    Posts
    139
    Downloads
    0
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Quote Originally Posted by ger21 View Post
    I believe that thee settings should be much lower, as your g-code consists of lots of straight segments, 0.1mm long.

    Also. do you have backlash comp enabled?
    I've lowered the settings closer to the original, mostly just wanted to see if problems went away with tolerances wide open. I don't have backlash compensation enabled, I've checked the ball nuts with and indicator and any backlash there is too small to measure reliably. Is there any other reason to enable this?


    Sent from my iPhone using Tapatalk



  14. #14
    Registered
    Join Date
    Jul 2007
    Location
    Canada
    Posts
    139
    Downloads
    0
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Quote Originally Posted by OlfCNC View Post
    Try increase the acceleration parameter on your axes to a value which your axes can handle as maximum.
    Try set the unify and additions in the CV larger, ie. values 100 for a test
    Set the linear and corners error according to what tolerances your job will allow.
    Acceleration is set to 2000 with a max velocity of 16000. These values let me jog the axis at full speed without shaking the machine. Any higher and the inertia from the gantry becomes an issue


    Sent from my iPhone using Tapatalk



  15. #15
    Member
    Join Date
    Jun 2015
    Location
    Sweden
    Posts
    943
    Downloads
    0
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Acceleration is set to 2000 with a max velocity of 16000. These values let me jog the axis at full speed without shaking the machine. Any higher and the inertia from the gantry becomes an issue
    Try set the unify and additions in the CV larger, ie. values 100 for a test
    Set the linear and corners error according to what tolerances your job will allow.



  16. #16
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    No, you don't want backslash comp enabled. I wanted to make sure that it wasn't the problem.

    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)


  17. #17
    Registered
    Join Date
    Jul 2007
    Location
    Canada
    Posts
    139
    Downloads
    0
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Quote Originally Posted by cygnus x-1 View Post
    If you have smoothing turned (in Fusion) on then something is not right because that code has no arcs in it. My guess is that your post is ignoring it for some reason. What post are you using? It would also help if you could post the Fusion project so we can see the operation settings. Having lots of tiny line movements can overload the controller's look ahead buffer and cause data starvation. This tends to cause sort of a stutter or chatter in the motion. Other than that the code looks ok.

    I'm thinking the thunk noise is something unrelated to the code, like an intermittent electrical connection, or even something mechanical. This is where you'll have to go around wiggling connectors and banging on things to see if you can induce the problem.


    C|
    I'm using the wincnc post processor. I tried using the cncrouterparts post as well as the mach 3 post but UCCNC tended to have lots of processing errors when I used them. Other guys using UCCNC recommended the win cnc post and it's been the most reliable, although sounds like it could be part of the problem. I don't know enough about post processors to evaluate their shortcomings.

    I would need curious to know why there are no arc sections in the code. The part it's machining was made from splines driving a lofted surface, which I know ends up as lots of little segments in a tool path, but tolerances are pretty loose on this, and I would have thought a large smoothing tolerance would let Fusion fit a few arc segments together to make a smooth path.


    Sent from my iPhone using Tapatalk



  18. #18
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Why are you not using the UCCNC post?

    Autodesk CAM | Post Library

    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)


  19. #19
    Registered
    Join Date
    Jul 2007
    Location
    Canada
    Posts
    139
    Downloads
    0
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Quote Originally Posted by ger21 View Post
    Why are you not using the UCCNC post?

    Autodesk CAM | Post Library
    I didn't know one existed. Last time I looked wincnc was recommended as the most compatible. I just downloaded 2 versions from the Fusion website. Do you know if there's any differences between the CNC drive version and the step craft version?


    Sent from my iPhone using Tapatalk



  20. #20
    Member ger21's Avatar
    Join Date
    Mar 2003
    Location
    Shelby Township
    Posts
    35538
    Downloads
    1
    Uploads
    0

    Default Re: Problems with Fusion 360 toolpaths

    Based on the release notes, I think they may be the exact same post?? Or they are updated together.

    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)


Page 1 of 3 123 LastLast

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

Problems with Fusion 360 toolpaths

Problems with Fusion 360 toolpaths