Page 1 of 4

Fusion 360 post processing

Posted: Sat Jun 13, 2015 2:54 am
by Lukesdad
Hello , I am new to the CNC world but have been a machinist for 23 years. I bought a shapeoko 3 and it runs great using makercam and carbide 3d. I've ran a few wooden signs to get a feel for the process and now it's time to get a little more serious so I can run prototype projects in wood and plastic. I have been using Fusion 360 for a few weeks and absolutely love it, but when I create a tool path and run the grbl post processor I get errors trying to run on the machine. Any advice on what I may be doing wrong? I have zeroed the machine, drew simple parts such as 3"x3" rectangles , still no luck , it doesn't like the g code fusion 360 is spitting out. Any tips would be greatly appreciated. And I am new to the computer/cam/g code side of things so speak slowly ;)

Re: Fusion 360 post processing

Posted: Sat Jun 13, 2015 3:27 am
by WillAdams
Which post-processor are you using?

According to http://www.shapeoko.com/forum/viewtopic ... 076#p41626 there’s a Grbl processor:
In terms of workflow, Fusion includes a very good GRBL v0.8 post-processor, so your workflow with Fusion 360 is simply this:
Build your model in the CAD editor -> Switch to CAM mode and construct your toolpaths -> Compile the NC file using the GRBL Post Processor -> Mill with Universal G-Code Sender.

Re: Fusion 360 post processing

Posted: Sat Jun 13, 2015 9:14 am
by Lukesdad
I am using the grbl.cps-generic GRBL selection from fusion 360 and Carbide Motion. I dug through posts and found that I had to delete g28 and that made it run basic rectangle and even an island. If I try to load anything with a curve in it I get "error in line xx bad arc format no I/K. I have hope, little by little. Should I try a different post processor from the list? Thanks for the response .

Re: Fusion 360 post processing

Posted: Sat Jun 13, 2015 11:38 am
by WillAdams
According to this: http://community.carbide3d.com/t/fusion ... =willadams

It should work:
Just uploaded a new CM V2 beta that works with Autodesk CAM.

Use the Mach3 post
Uncheck "Use Radius" in the post processor

Re: Fusion 360 post processing

Posted: Mon Jun 22, 2015 4:25 am
by Lukesdad
Back from another hitch at work and had time to play. This worked great, Thank you for your help!

Re: Fusion 360 post processing

Posted: Mon Jul 27, 2015 12:54 am
by gradymorgan
Where is the "Use Radius" button? I've tried selecting grbl.cps and mach3mill.cps, but cannot import the output of either of these into Carbide Motion. I haven't been able to find any post processor options, though, and haven't been able to try unchecking the "use radius" button.

Re: Fusion 360 post processing

Posted: Sat Aug 01, 2015 3:58 am
by OttoPilot
gradymorgan wrote:Where is the "Use Radius" button? I've tried selecting grbl.cps and mach3mill.cps, but cannot import the output of either of these into Carbide Motion. I haven't been able to find any post processor options, though, and haven't been able to try unchecking the "use radius" button.
Once you select 'post process' you'll see this dialog box appear.

Image


Has anyone found a solution to canned cycles in Fusion 360?

I've been posting my drill steps in 'generic grbl', and my milling in 'generic mach3'...but I'm getting sick of having to post and run two separate files.

Re: Fusion 360 post processing

Posted: Sat Aug 01, 2015 1:41 pm
by heathenx
I think they advise you to turn g28 off too. I did. I use HSM Express in Inventor which is nearly the same as Fusion without the 3D.

Why grbl for drilling and mach for milling? Does Carbide not recognize something? I haven't tried drilling yet.

Re: Fusion 360 post processing

Posted: Sat Aug 01, 2015 3:34 pm
by OttoPilot
That screen is actually from HSM Express (they use the same post screen :D ).

Using the Mach3mill post processor works great for milling but uses 'canned cycles' (G81 for peck drilling etc) which aren't compatible with Grbl and throws an error.

If you use the grbl post processor it converts the drilling into simple G01 linear commands, but for for milling it throws the 'bad arc format, no i/k' error.

So I've been posting two files, one with the grbl post processor for spot drilling, and one with the generic Mach3mill post for all the milling ops.

I've considered using a complete grbl post (with drilling and milling all included) along with universal g-code sender (UGS), but UGS doesn't appear to allow tool changes; so I'm back to posting and running two files; which is what I'm trying to avoid.

I need to figure out a way to either edit the grbl post processor to fix the arc error, or edit the mach3 post to eliminate the canned cycles...I just have NO idea how to begin.

Re: Fusion 360 post processing

Posted: Sat Aug 01, 2015 3:51 pm
by heathenx
Ah! Got it! Thanks for the explanation.