Hello The toolpath created by Fusion 360 sounds good but the one shown in Control is really weird in some places. I opened the same GCode in ncviewer and the toolpath seems ok in it so I guess it may be an issue in Control to be checked? Code and pictures attached
The viewer does a best-effort but can fail on some arcs etc It will run fine even if the viewer failed at it
Ahh sorry, yes indeed. In this case though David reported it a couple days ago, just haven't gotten round to fixing the Parser yet. sorry! Please do post your file and I'll give it a test while I work on the code
This is sorta similar problem: Using Vetric Desk Top Pro and OB Control with OB Black Box. Making an inlay of letters cut out the pockets just fine, started running the inlay and I get two errors. Here is a short section of code: T1 G17 G20 G90 G0Z0.8000 G0X0.0000Y0.0000 M3S16000 G4 P1.8 G0X1.5140Y1.0766Z0.2000 G1Z0.0000 G1Z-0.0353 G1Z-0.0367 G1Z-0.0382 G1Z-0.0397 G1Z-0.0411 G1Z-0.0426 G1Z-0.0441 G1Z-0.0455 G1Z-0.0470 G1Z-0.0485 G1Z-0.0499 G1Z-0.0514 G2X1.6240Y1.3238I0.0925J-0.0595F30.0 G1X1.7140 First problem is a missing feed rate for line 10 (G1X1.7140) easy to fix I just added F35.0 and machine continues on to line 23 (G2X1.6240Y1.3238I0.0925J-0.0595F30.0) an error code of 33 Motion command target is invalid. Where are these errors originating? Seems like 3 possible places Desk Top Pro, Black Box or Control. How do I fix this? PS Running simulation on Control looks just fine no stops occur.
Check Max Travel settings in Grbl Settings Check that machine is homed and zeroed properly before starting the job Check that Job fits in the working envelope of the machine Have a read through the Grbl Wiki at github.com/gnea/grbl/wiki
Also check that you are fully up to date with the Vectric software. If you upgraded recently to version 10.5 there have been problems with several post processors - missing feed rates and error 33 on arcs and spiral ramps. Which post processor did you use? The latest patch (V10.505) claims to have fixed those issues. Alex.
I think you are using the wrong post processor as GRBL Gcode should not include a T1. Also, the arc parameters are incorrect arc from G0 X1.5140 Y1.0766 Z0.2000 to G2 X1.6240 Y1.3238 I0.0925 J-0.0595 does not define the correct center for those endpoints, that is what error 33 means. this is what bCNC displays for that arc (it tolerates the errors but displays the wrong thing as a result). the blue highlighted segment is supposed be be the arc from bottom to top, ie the straight line is NOT correct. The are many arcs than can go from X1.5140 Y1.0766 to X1.6240 Y1.3238 it all depends where the center is defined by the I and J parameters, but these ones are wrong. Here I have plotted the given points... clearly there is no arc that fits between those points with that center. So the problem is in Vectric or in the Vectric post.
That did it, downloaded the patch and it ran fine. There may be an overshoot on the depth of cut. I will run a test tomorrow and see, if so I will send a note to Vetric. Thank you for the help.
