URGENT 4th Axis Post Processor support for APSX - Spyder CNC

[CriticalInnovations]

I have downloaded the post processor for my CNC from Fusion 360's website. When posting a 3 axis part it works perfectly. When I ad a tool rotation to utilize my 4th axis I get error messages.

I have included these items . . .

my post processor

a screen shot of the errors

a sample file that has a 3 axis hole being milled and a second line including the tool rotation.

post with the 3 axis that worked 

post with the tool rotation that didn't work

Please let me know if you can edit my PP

Thank you

[seth.madore · Accepted solution]

Couple of things going on:

1) Your post processor is NOT setup for 4-axis motion.

2) There is language in the post that prevents you from using "Clearance Height" as the retract position. Use " G28" instead:

All that said; I edited the post for you and it's now posting out 4 axis code. Simple edit to do, just needed to change a few bits and off we go!

%
(1001)
(A TOP ROUGH OUT)
(T2  D=0.125 CR=0. - FLAT END MILL)
N10 G90 G94 G17 G91.1
N15 G20
N20 G28 G91 Z0.
N25 G90
(2D ADAPTIVE2)
N30 T2 M6
N35 S20000 M3
N40 G0 A0.
N45 G0 X-0.0566 Y-1.582 Z1.4
N50 G0 Z1.2
N55 Z1.102
N60 G3 X0.0566 Y-1.618 Z1.0857 I0.0566 J-0.018 F25.
N65 X-0.0566 Y-1.582 Z1.0694 I-0.0566 J0.018
N70 X0.0566 Y-1.618 Z1.053 I0.0566 J-0.018
N75 X-0.0566 Y-1.582 Z1.0367 I-0.0566 J0.018
N80 X0.0566 Y-1.618 Z1.0204 I0.0566 J-0.018
N85 X-0.0566 Y-1.582 Z1.0041 I-0.0566 J0.018
N90 X0.0566 Y-1.618 Z0.9878 I0.0566 J-0.018

[CriticalInnovations]

The Post Processor works, Thank you!!! I had to switch that the A axis rotatation on the Y axis instead of X but thanks to this forum, I already knew how to do that!!!

[seth.madore]

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

That is the current configuration for an X axis machine. Read this article on how to configure it to match your needs

[CriticalInnovations]

I am now looking to do a multi axis rotary machining and when I post the process I get an error that reads, "REWIND: Rewind of machine is required for simultaneous multi-axis toolpath and has been disabled."

I have searched through the .nc program and it doesn't appear to have any where to make this statement (True) 

I believe it may need to be added, but I don't know where to add it in the script. Please assist.

I have attached my Post Processor again.