Fixed: How do I export manufacturing gcode from Fusion 360 for the mini cnc?

[Calin (Calin Mocanu)]

Hi, I tried to machine a 3D model directly from Fusion 360. I downloaded the tools library from the Mini CNC page and set the post processor to LinuxCNC (EMC2), so I think I followed the proper steps.

But I’m getting these weird errors, and I think they’re caused by a misconfigured setting somewhere that specifies how arcs are represented in gcode. Do you know what these mean? (@Kyle do you know?)

“Radius to end of arc differs from radius to start”

and if I click the checkbox for “Radius arc” on the “post process” page on Fusion 360 the error on Linux CNC changes to:

“Arc radius too small to reach end point”. See the screenshots (with my phone)

[Kyle (Kyle Barker)]

Can you post the full gcode file with Radius arc off? The problem is that arcs (G2 and G3) are specified as ending coordinates and intermediate point IJK (when R mode is off). These are subject to rounding errors and different systems have different tolerances. LinuxCNC is not happy interpolating that curve for some reason.

[Calin (Calin Mocanu)]

Ok I turned radius arcs back off, line 20 with the error Radius to end of arc differs from radius to start:

N65 G3 X7.952 Y26.04 Z2.431 I-0.163 J0.986 F480.

Full g code is a few mb, but it starts like this:

%
(WRIST GUIDE PIECES)
(MACHINE)
(  VENDOR ISEL)
(  MODEL CPM 2018)
(  DESCRIPTION SLMS SMALL CNC)
(T18  D=2. CR=0. - ZMIN=-3. - FLAT END MILL)
N10 G90 G94 G17 G91.1
N15 G21
N20 G53 G0 Z0.
(ADAPTIVE1)
N25 T18 M6
N30 S19000 M3
N35 G54
N40 G64 P0.1 Q0.1
N45 G0 X7.274 Y24.514
N50 G43 Z15. H0
N55 G0 Z5.
N60 Z2.5
N65 G3 X7.952 Y26.04 Z2.431 I-0.163 J0.986 F480.
N70 X6.284 Y26.058 Z2.362 I-0.84 J-0.54
N75 X6.928 Y24.521 Z2.293 I0.827 J-0.556
N80 X8.082 Y25.72 Z2.224 I0.183 J0.979
N85 X6.526 Y26.304 Z2.155 I-0.97 J-0.22
N90 X6.607 Y24.646 Z2.086 I0.586 J-0.803
N95 X8.095 Y25.376 Z2.017 I0.504 J0.855
N100 X6.836 Y26.452 Z1.948 I-0.983 J0.124
N105 X6.348 Y24.871 Z1.879 I0.276 J-0.951
N110 X7.99 Y25.049 Z1.81 I0.763 J0.629
N115 X7.177 Y26.485 Z1.74 I-0.879 J0.45
N120 X6.182 Y25.171 Z1.671 I-0.065 J-0.984
N125 X7.781 Y24.779 Z1.602 I0.928 J0.33
N130 X7.508 Y26.4 Z1.533 I-0.67 J0.721
N135 X6.129 Y25.508 Z1.464 I-0.396 J-0.899
N140 X7.493 Y24.597 Z1.395 I0.981 J-0.007
N145 X7.788 Y26.208 Z1.326 I-0.382 J0.903
N150 X6.194 Y25.841 Z1.257 I-0.676 J-0.708
N155 X7.162 Y24.525 Z1.188 I0.917 J-0.34
N160 X7.986 Y25.933 Z1.119 I-0.051 J0.975
N165 X6.368 Y26.131 Z1.05 I-0.874 J-0.433
N170 X6.827 Y24.569 Z0.981 I0.743 J-0.63
N175 X8.078 Y25.608 Z0.912 I0.284 J0.931
N180 X6.63 Y26.344 Z0.843 I-0.966 J-0.108
N185 X6.528 Y24.725 Z0.774 I0.481 J-0.843
N190 X8.053 Y25.273 Z0.705 I0.582 J0.775
N195 X6.947 Y26.454 Z0.636 I-0.941 J0.227
N200 X6.302 Y24.973 Z0.567 I0.164 J-0.953
N205 X7.916 Y24.967 Z0.498 I0.809 J0.528
N210 X7.282 Y26.449 Z0.429 I-0.804 J0.533
N215 X6.174 Y25.282 Z0.36 I-0.17 J-0.948
N220 X7.683 Y24.728 Z0.29 I0.937 J0.219

[Calin (Calin Mocanu)]

This is the post screen in my fusion 360

[Kyle (Kyle Barker)]

Not sure why we weren’t having this issue before but I loaded your gcode with the g43 tool length compensation line (20 or N50) commented out and Linux CNC was happy. We can always do a custom post but it’d be nice if there was a GUI option.

@CNCtechs

[Calin (Calin Mocanu)]

Awesome, I’ll try it again when I get the chance.

[Kyle (Kyle Barker)]

Just confirming that this fixes the problem Nice to see your PTFE carpal tunnel last night!

[Calin (Calin Mocanu)]

Yes it did, and I learnt how to adjust the adaptive clear parameters to make some deeper cuts in the plastic, cause it was so soft 3hours -> 30min. Thanks for the tip!