Error code when posting to Carbide 3d Nomad

[williespoke]

Recently I've been generating a lot of toolpaths from complex vector geometries imported into fusion 360 from vector image programs like inkscape/illustrator. Fusion posts the code no problem, but every once in a while I get an error:

"Error (5): GRBL Error: The motion command has an invalid target. G2, G3, and G38.2 generates this error, if the arc is impossible to generate of if the probe target is the current position."

Why would fusion program a toolpath arc that is impossible to generate?!?! Turning off "smoothing" and decreasing the spline fidelity tolerance seems to help a bit, but not entirely.

What's going on here? How can I fix this?

Thanks!

[kate.raskauskas]

Hi @williespoke,

Can you please attach one of the files you're having trouble with so I can take a look at the toolpaths? Also, just to double check - you're importing these vector geometries and directly generating toolpaths from them, right? (That is, there's not "native" geometry that was created in Fusion 360 like a sketch or a model or anything.) And you're using the generic Carbide 3D post for Fusion?

Thanks!

[williespoke]

The error occurs in the attached file at (or around) line 12011 of 105509.  I'm inserting a 2d svg file from inkscape, extruding a solid model from the imported geometry, and then creating 3d toolpaths from the model.

I am using the generic Carbide 3d post.

Thanks a lot!

Willie

[kate.raskauskas]

Hi Willie - 

Thanks for the code and the screencap! It would be great though if you could share the f3d file with me so I can see the toolpath settings/selections as well. (Here's a run through of how to do this in case you need it)

Thanks!

[williespoke]

Here ya go!

I hope i did that right 😉

http://a360.co/2tqLnKi

[kate.raskauskas]

Perfect, thanks! I'll take a look and let you know what I find out 🙂

[HughesTooling]

The arc that's giving the error is only 0.001" from start to end and only 0.001" radius. Rads this small give lots of controls problems because 4 decimal places is not enough for something this small! 

On the post dialog is there a setting for minimum radius and minimum cord length, try setting them to 0.025, these sizes are in mm and no the document settings so even if you increase them to 0.05mm that's only 0.002". I've had to change these defaults from 0.01mm for a couple of my controls, some controls are more tolerant.

Mark

[williespoke]

Thanks! I'm giving this a shot right now

[williespoke]

This doesn't seem to have solved the issue

[williespoke]

Ok, I kept increasing the "minimumChordLength" "minimumCircularRadius" and "tolerance" settings until the alarm disappeared.  I landed on 0.15, 0.15, and 0.1 for those values, respectively. This seems to have finally solved the issue.

[HughesTooling]

---

@williespoke wrote:

 I landed on 0.15, 0.15, and 0.1 for those values, respectively. This seems to have finally solved the issue.

---

You have 3 numbers, which 3 parameters have you set? I only change the 2 shown in blue in the picture above.

Mark

[jphilips6LGA9]

---

@williespoke wrote:

Ok, I kept increasing the "minimumChordLength" "minimumCircularRadius" and "tolerance" settings until the alarm disappeared.  I landed on 0.15, 0.15, and 0.1 for those values, respectively. This seems to have finally solved the issue.

---

This worked for me.  Thank you!   

[clutterlabs]

I would like to report that none of the suggested post process settings worked for me in the case of a 2D adaptive clear toolpath. I reset the values to default and turned OFF "Both Ways" under Passes tab. I turned in initially for faster clearance with both climb and conventional milling.