Post processor 'onOpen' error with Flow CAM operation in Fusion 360

[Florian Paproth]

Hello, 

the normal CAM Operations are no problem and now I understand so setup them but when I try 'Multi Axis Milling' in a Flow Operation I am not able to generate the g-code for it with the given Pocket NC post processor. 

Here is the log from the Fusion trying to generate the tool path with the PocketNC Post

Information: Configuration: Pocket NC

Information: Vendor: Pocket NC

Information: Posting intermediate data to '/Users/florian/Desktop/ChessTowerBodyfine.ngc'

Error: Failed to post process. See below for details.

...

Loading locale from '/Users/florian/Library/Application Support/Autodesk/webdeploy/production/742b51de82fb690ad30c10d35d2e983ab4a4fc6a/Autodesk Fusion 360.app/Contents/Libraries/Applications/CAM360/Data/Translations/german_de.xml'

Start time: Thu Feb  6 17:15:42 2020

Post processor engine: 4.55.0 0

Configuration path: /Users/florian/Autodesk/Fusion 360 CAM/Posts/pocket_nc.cps

Include paths: /Users/florian/Autodesk/Fusion 360 CAM/Posts

Configuration modification date: Tue Aug 20 12:12:40 2019

Output path: /Users/florian/Desktop/ChessTowerBodyfine.ngc

Checksum of intermediate NC data: 4ecd20c859c085ce26cf48662ba800b2

Checksum of configuration: 7d3d00b90003915574c3ccbe31464efc

Vendor url: http://www.pocketnc.com/

Legal: Copyright (C) 2012-2018 by Autodesk, Inc.

Generated by: Fusion 360 CAM 2.0.7421

...

Fehler: Failed to invoke 'onOpen' in the post configuration.

^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^

Fehler: Failed to invoke function 'onOpen'.

Fehler: Failed to execute configuration.

Stop time: Thu Feb  6 17:15:42 2020

Post processing failed.

My Setup works fine with the other CAM operations.

But when I try to use the Flow operation with Multi Axis than it don't work. 

Any ideas? 

Here is the Link to the Project

https://a360.co/39hyIgO

Best regards 

Florian

[Graham Stabler]

The x and y axis of the WCS are the wrong way around. When I fixed this it was fine, for operations from the top it would not matter. With the table flat z points at the spindle and x should point to the right as seen by the spindle.

Also the origin of the WCS should be at the end of the sketch line (~21.3mm long) coming from the table. 

The error was actually related to the A axis trying to point too far downwards I think because of the coordinate system. The error I saw was:

Error: Tool orientation is not supported for available machine axes.

Error at line: 1

Cheers,

Graham 

[Florian Paproth]

Thank you it worked. After I tried several setup variants yesterday with you hint it fixed it. 

Also I recognized that the cam failed, when I increase the 'Maximum tilt angle' over 115°. When I do that the simulation seems fine but it won't generate the post. But 115° works fine for that job. 

Thanks again for the help.

[Graham Stabler]

No problem and it was handy because I forgot you could do 5-axis flow, it used to be in the multi-axis section I think and they moved it because a lot of people didn't realize it could be used for 3-axis.

Cheers,

Graham