Skip to content

Documentation

Jump to bottom
Pascal Roobrouck edited this page Sep 5, 2016 · 11 revisions

How to install a Custom Post Processor in Autodesk Fusion360 ?

Download the .cps file, then move it to a proper location on your machine. It does not have to be in a certain folder, from the Fusion Post DialogBox you can refer to its location. Fusion will then remember this setting. After setting the path, Fusion will list all PostProcessors from that folder and then you can choose the one you want to use. You could store several variants in the same folder, and select the one you need for a specific job, eg if you have different machines with different capabilities

Adding Custom Post Processor

No Toolchanges

For the time being, the GRBL-controller and the CNC-machines using it (Openbuilds, Inventables, Shapeoko, X-Carve) don't support automatic toolchange. So it makes no sense to post toolchange-code. On the other hand it makes sense to check that you've not accidentally posted multiple operations in 1 file, needing different tools.

Return to Home after all operations are completed

When the job is finished, you need the machine to move away from your workpiece so you can easily inspect it, check measures and finally remove it. Although GRBL supports G28, you need to be sure a safe location has been set before.. After some study of G28, I concluded that G53 is actually simpler and more reliable. The Post Processor adds following blocks at the end :

  • retract the spindle : rapid up to machine Z-3
  • shut down spindle (+ short wait for spindle to actually stop)
  • rapid back to machine X-10 Y-10

The reason to move to -10, -10, -3 is that going to 0, 0, 0 will possible trigger the limit switches. These safe X,Y,Z-positions can be set in the Parameters-box when posting.

Setting Safe Location

This will result in the following G-Code at the end of all operations :

  • G53 G0 Z-3 (Move spindle up to top of machine - 3mm)
  • M5 (Stop spindle)
  • G4 P0.8 (Wait 0.8 sec for spindle to come to a stop)
  • G53 G0 X-10 Y-10 (Move machine to X-10 Y-10 position, machine coordinates) Note : due to so-called 'Modal' way of handling G-Code, Fusion will not write G-Code for modes which are already in effect. For this reason it may seem that G0 is missing. This is because G0 is already in effect, and does not need to be repeated.

Clone this wiki locally