CNC Milling - IJK as absolute NOT incremental

[Anonymous]

Good Morning,

I'm currently using a Forest Scientific CNC Router at my high school to create a Poker Table Chip Tray in my Materials Engineering Class. 

I built out the model and the tool path in Fusion 360 and tried to run it on our CNC. One of the three of my g-codes work. The problem that I keep encountering is "Error code 1332 on line 208: The vector to the center defines an invalid arc. The arc cannot be drawn from the beginning point to the ending point with the center as specified". 

Based on what I've researched on the internet, it seems the problem has something to do with Fusion 360 because Fusion generates the "IJK" coordinates in an incremental mode rather than an absolute mode. 

Can anyone offer some guidance on this matter? I don't know how to fix these problems myself and I would greatly appreciate any feedback and support that would help me solve this issue.

Please see attached the F3D file of the part, one of the posts that I generated & the CPS file that was used to generate the post.

I would appreciate your feedback!

Patrick.

[andrea.amilo]

Hello @Anonymous ,

to set circular interpolation using IJK in absolute, I think you have to remove the calculation at lines 740, 743, 746, 756, 761 and 766 in onCircular function of your postprocessor. You need to remove - start.x or - start.y or - start.z .

You will find 12 occurrences to be modified. 

The following picture shows you a comparison between your original post (on the left) and the modified one :

I hope this could help you.

Please test it carefully and let me know.

[Anonymous]

Thank you @andrea.amilo for getting back to me so soon.

Sorry I didn't get back to immediately. I did as you said by removing the 12 occurrences that you pointed out and made new g-codes with the edited CPS file in the Fusion 360 Post Processor. Unfortunately, when I tried to open the new G-Codes on the CNC, it came up with the same error messages same as before. I'll attach the edited CPS file just incase I did something wrong. Do we have any other ideas for might have caused this error?

[andrea.amilo]

Hello @Anonymous ,

it seems that you've made the correct modification. I don't know why you still have the error message running circular moves.

In my opinion you can solve this situation removing all the arcs and write only linear moves.

If you want to try this modification, you have to modify line 34 of your postprocessor as follow :

allowedCircularPlanes = 0; // no circular motion allowed

Please test it carefully and let me know.

[mrnfr]

good morning,

i am getting the same error using the autodesk basic 3-axis cnc machine and forest scientific post in fusion 360 cam. did you solve this problem? please, advise.  thanks.

[jmusickQ7YSS]

I know this post is several years old, but I ran into the same exact issue today and figured out an easy solution that wasn't provided above. Hopefully this helps folks who run across this issue in the future.

First, make sure you have the Forest Scientific Post Processor downloaded and installed on Fusion. Here's a video to help with that:  https://www.youtube.com/watch?v=eY8e4un-wm0

Next, when running the post processor, make sure to choose the Forest Scientific Router processor. In settings (in the post processor window, also called NC Program) at the bottom right, in the "Built In" menu unclick the box next to (Built-in) allow helical moves. (see attached image). This solved the problem for me. I hope it does for you!

This box should be empty.