Not pausing for manual tool change using fusion 360 for masso (solved with correct post p)

CAD (Design) Software Fusion 360
1

I just installed the OneFinity tool setter, which mostly went according to plan/vidoes.

However, when run a job with multiple tools it will pause before a new tool is required, but it doesn’t move to the tool change position I set in the F1 screen (Tool Changer => Manual Tool Change => enable x, y, z and set coordinates). It simply pauses for a bit (rotation stops), then spins back up and proceeds with the job even though I haven’t been able to change the tool.

Also, the screen never prompts me to change tools. They do have different indices in Fusion.

What am I missing? Generating .nc files with Fusion 360, all worked as expected until I installed the Tool Setter. NC file I’m testing with is attached.
InsertTest.nc (60.4 KB)

2

Looking at the gcode, the M5 - which appears first - and T# are on separate lines.

Masso is looking for Tool Number first then M5 and on the same line…

For example: T1 M6

Which post processor from Autodesk are you using?

https://docs.masso.com.au/cam-post-processors/fusion-360

3

Not sure if this helps but, if you don’t have your tool numbers in Masso that match you CAD software there will be issues. In Vcarve, I experienced similar issues.

4

Thanks @Mick427 , that was an update I had to make but even after matching numbers I was still not getting proper prompts for tool changes.

5

I see you are quite busy answering tool change questions here @TMToronto !

I had been using the Onefinity 2021 pp. Changing to the Masso .cps you linked to does finally give me prompted tool changes! It’s a bit clunky as there are extra , unprompted steps:

  • Operation runs
  • Spindle stops and tool withdraws, but no prompts
  • Hit Cycle Start
  • Tool moves to load location and screen prompts for change
  • Hit Cycle Start after changing tool
  • Tool properly registers at Setter then proceeds
  • …

So I wish I could skip that first Cycle Start hit, but at least I can run multiple operations from one NC file and utilize the Tool Setter.

Progress!

6

this fusion post processor is for Buildbotics controllers and not for the Masso controller.

7

There may be an Optional Stop (M1) causing this.
Torn off Optional Stop - press it at top of screen to toggle On/Off

8

That setup was working fine until I installed the Tool Setter. Thanks for the info.

9

Spot on @TMToronto, that was the issue. You ever make it to Seattle I owe you a beer ;-}

10

I had this same issue but when i turned off optional stop it worked for the first bit change but not the second?

11

Not sure if others are still having this issue, I found a fix for this, as I was getting frustrated with it not working. Unchecking the manual tool change box in the tool library settings changed the gcode to include the M6 code when a tool change was required. Works on both the onefinity masso and masso post processors

Snip - Tool Library
Snip - Tool Library583×388 21.9 KB