NEED HELP WITH FANUC 5 AXIS POST PROCESSOR

[wgr_eng]

Hello 

I just started using Fusion 360. I need help with the post processor. 

I have a sample code that works with my machine using another cam package.

I want some help making changes.

Thank you 

[wgr_eng]

Information: Size of intermediate NC data: 19.1kb

Debug: Loading intermediate NC data from 'c:\Users\pmt\.vscode\extensions\autodesk.hsm-post-processor-3.2.2\res\CNC files\Milling\5x Simultaneous\swarf.cnc'.

Debug: Loading intermediate NC data as CNC.

Debug: Intermediate NC data loaded.

Debug: Number of NC records: 617

Debug: Number of NC sections: 1

Debug: Number of tools: 1

Debug: NC record build time: 00:00.153

Debug: NC record memory usage: 85.4kb

Debug: overriding property: programName=1005

Debug: overriding property: unit=0

Debug: overriding user-defined property: programName=1005

Debug: overriding user-defined property: unit=0

Information: property: writeMachine=true [true]

Information: property: writeTools=true [true]

Information: property: preloadTool=true [true]

Information: property: showSequenceNumbers=true [true]

Information: property: sequenceNumberStart=10 [10]

Information: property: sequenceNumberIncrement=5 [5]

Information: property: optionalStop=true [true]

Information: property: o8=false [false]

Information: property: separateWordsWithSpace=true [true]

Information: property: allow3DArcs=false [false]

Information: property: useRadius=false [false]

Information: property: forceIJK=false [false]

Information: property: useParametricFeed=false [false]

Information: property: showNotes=true [true]

Information: property: useSmoothing=true [true]

Information: property: usePitchForTapping=false [false]

Information: property: useG95=false [false]

Information: property: useG28=true [true]

Information: property: useG54x4=true [true]

Information: property: useSubroutines=false [false]

Information: property: useFilesForSubprograms=false [false]

Information: property: useSubroutinePatterns=false [false]

Information: property: useSubroutineCycles=false [false]

Information: property: useRigidTapping='yes' ['yes']

Information: property:*programName=1005 [undefined]

Information: property:*unit=0 [undefined]

Debug: Opening temporary NC file 'C:\Users\pmt\AppData\Local\Temp\debuggedfile.nc'.

Information: Configuration: FANUC

Information: Vendor: Fanuc

Information: Posting intermediate data to 'C:\Users\pmt\AppData\Local\Temp\debuggedfile.nc'

Information: Elapsed time: 00:00.983

Information: Size of output: 31.5kb

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

...

Code page changed to '1252  (ANSI - Latin I)'

Command-line: C:\Users\pmt\AppData\Local\Autodesk\webdeploy\production\d329faf365c350668f1b0d009520835a9e1834a8\Applications\CAM360\post.exe --noeditor --debugall --shorten 50000 --property unit 0 --property programName 1005 "c:\Users\pmt\Desktop\5 AXIS\HSMWORKS POST PROCESSOR\G250 working post FANUC\making edits COPY\fanuc_31I_EDITING.cps" "c:\Users\pmt\.vscode\extensions\autodesk.hsm-post-processor-3.2.2\res\CNC files\Milling\5x Simultaneous\swarf.cnc" C:\Users\pmt\AppData\Local\Temp\debuggedfile.nc

Start time: Monday, August 3, 2020 7:08:08 PM

!DEBUG: 1 fanuc_31I_EDITING.cps:24

Code page changed to '20127 (US-ASCII)'

Post processor engine: 4.5689.0

Configuration path: c:\Users\pmt\Desktop\5 AXIS\HSMWORKS POST PROCESSOR\G250 working post FANUC\making edits COPY\fanuc_31I_EDITING.cps

Include paths: c:\Users\pmt\Desktop\5 AXIS\HSMWORKS POST PROCESSOR\G250 working post FANUC\making edits COPY

Configuration modification date: Monday, August 3, 2020 7:06:00 PM

Output path: C:\Users\pmt\AppData\Local\Temp\debuggedfile.nc

Checksum of intermediate NC data: 1b69f9128db4b9d92e87b05982c55f10

Checksum of configuration: f715ed01dffb1a58d8795c6dba8ffc80

Vendor url: http://www.fanuc.com

Legal: Copyright (C) 2012-2020 by Autodesk, Inc.

Generated by: Fusion 360 CAM 2.0.8156

...

Error: REWIND: Rewind of machine is required for simultaneous multi-axis toolpath and has been disabled.

Stop time: Monday, August 3, 2020 7:08:09 PM

Post processing failed.

[wgr_eng]

So my 5 Axis machine Hardinge GX 250 5AX has limits C (0,360) & A (-120, 30).

My other software generates the correct angles but Fusion outputs A angle beyond machine limts.

The angles should be as below  

A -45 C 180

A -45 C 360

How do I add this logic to my post processor.

[wgr_eng]

@Anonymous 

@Seth.Madore

[boopathi.sivakumar · Accepted solution]

Hi @wgr_eng 

It seems you have to set the kinematics properly

  if (true) { // note: setup your machine here
    var aAxis = createAxis({coordinate:0, table:true, axis:[1, 0, 0], range:[-120, 30], preference:0});
    var cAxis = createAxis({coordinate:2, table:true, axis:[0, 0, 1], cyclic:true, range:[0, 360], preference:0});
    machineConfiguration = new MachineConfiguration(aAxis, cAxis);

    setMachineConfiguration(machineConfiguration);
    optimizeMachineAngles2(0); // TCP mode
  }

For your machine it should be something like above

you cannot use cyclic for both the axis. Cyclic only applies to axis which has the true cyclic motion (C axis) 

Kindly check and see now everything will be in the limits

[wgr_eng]

@boopathi.sivakumar 

The angles should be A -45 C 0 & A - 45  C 180. 

I changed the C axis : [0, 0, -1] and it gave me the right code. 

Correct me if I'm wrong.

Thank you

[boopathi.sivakumar · Accepted solution]

It depends on the how the machine is set to do... If you need to go other way you can use -1 or 1 depends.. So if -1 works that's absolutely fine

Hope it helps