4 Axis Postprocessor Fusion 360

[PCSM-CNC]

Hello Forum, hello Supportteam.

I use the MK3/4 controller and for drawing and cam Fusion360.
I got a postprocessor whitch works realy good but i can not use the 4 Axis.
There is en error when i create the gcode.

Anybody have an idea or an postrocessor?

If somebody need, i can upload the pp whitch i use.
Also i have a second pp without use the G43 gcode.
It is very helpful for generate without G43.

Regards from Germany

Similar Threads:

• 4th Axis and Fusion 360
• Solidcam five axis postprocessor editing (by modifiying 3 axis post)
• Need Help!- CNC Fusion Z Axis Question
• Need Help!- CNC Fusion X2 kit - possible to swap over X-axis?
• Need Help!- X2 CNC Fusion #4 Kit Y-axis Mod

[PlanetCNC]

Which error do you get?

[PCSM-CNC]

Here is the Errorpost

Information: Configuration: Planet CNC USB
Information: Vendor: Planet CNC
Information: Posting intermediate data to 'U:\Fertige G Codes\Tests\1001.tap'
Information: Total number of warnings: 1
Error: Failed to post process. See below for details.
...
Loading locale from 'C:\Users\Alex\AppData\Local\Autodesk\webdeploy\pr oduction\72ff341930ac680f0fc073441e10ee045a3f129c\ Applications\CAM360\Data\Translations\german_de.xm l'
Code page changed to '1252 (ANSI - Lateinisch I)'
Start time: Saturday, January 06, 2018 8:55:57 PM
Code page changed to '20127 (US-ASCII)'
Post processor engine: 4.2.1 41684
Configuration path: C:\Users\Alex\AppData\Local\Autodesk\webdeploy\pro duction\1c8eda3d042f236f121d6fb4e850f0621b6f700b\A pplications\CAM360\Data\Posts\planetcnc.cps
Include paths: C:\Users\Alex\AppData\Local\Autodesk\webdeploy\pro duction\1c8eda3d042f236f121d6fb4e850f0621b6f700b\A pplications\CAM360\Data\Posts
Configuration modification date: Friday, December 30, 2016 10:30:15 AM
Output path: U:\Fertige G Codes\Tests\1001.tap
Checksum of intermediate NC data: 25a988730a3aff5a5b45ca592ec9a177
Checksum of configuration: eb02babaea990edbf614efdf01b66663
Vendor url: GameSpy: PC Games, Reviews, News, Previews, Demos, Mods & Patches
Legal: n/a
Generated by: Fusion 360 CAM 2.0.3797
...
Warnung: Work offset has not been specified. Using G54 as WCS.
Fehler: This post configuration has not been customized for 5-axis simultaneous toolpath.
^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^ ^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^^
Fehler: Failed to execute configuration.
Stop time: Saturday, January 06, 2018 8:55:57 PM
Post processing failed.

[daniellyall]

That means the A axis and B or C is not turned on in the post processor.

It's under on open you change it from false to true and set what Axis you wont on extra to a axis

This is what the code looks like that needs changed

if (false) {
var aAxis = createAxis({coordinate:0, table:true, axis:[-1, 0, 0], cyclic:true, preference:1});
machineConfiguration = new MachineConfiguration(aAxis);

[PCSM-CNC]

Here is the used Pp

You have only change ending .txt to .cps

[daniellyall]

Done it did it with A and B axis

[PCSM-CNC]

Awesome.

What was the reason for the error?

I try it so soon as possible

Now i need the new license for TNG Software.
Yesterday i switched from old version to TNG.
It`s tricky but slowly it will run.
Now waiting for the license and then i can try the Pp.

Thank you Daniel for your Help.

Best regards from late night germany :-)
Alex

[daniellyall]

What was the reason for the error? The A axis was set to be off in the post it's the way most posts are that it's off by default and I added the B axis for fun, if you needed it, it cab=n be changed to c easyily.

[PCSM-CNC]

Dear Daniel.

The change in Pp works awesome.

Thank you.
Now i can use the 4th rotaryaxis

[daniellyall]

Good stuff thanks for the confirmation that it works.