Fusion 360 post processing with the post processor from the sticky thread

Hi, 
So i got my machine up and running i just imported the pp for Fusion360 from the sticky thread. 
I want to start finetuning the settings for each Material i use. 
As far as i understood the complete z axis stuff is handled by plasmaC except for Kerf width, the lead in lead out and compensation.

Is the feed rate setting from plasmac being used since my generated g code has " F#<_hal[plasmac.cut-feed-rate]> " ? 
Does Fusion handle any other settings except of the tool dimensions and the compensation ?

Any help would be much appreciated.

Greetings

So i did sort it out. 
As phillc stated the feedrate will be handled via plasmac using plasmac and the Fusion PP on the Sticky thread. 
I did modify the postprocessor as i did not want the material to be chosen via Gcode since i want to have the same file and chose the material in plasmac. I did not want to have to delete the M190 P# command everytime i postprocess something. 

Second thing i modified in the PP was the Centerpunch Feature as the M3 command used by the PP does not work for my machine (Linuxcnc 2.8.4 plasmac + Mesa7i96s with a Cebora Plasma Prof 52)  i changed the M3 command so it uses the Spindle rotate clockwise command instead of counterclockwise and now the centerpunch Feature is working again.(Using the original PP from sticky my machine does the centerpunch movements but like 5cm in the air the z axis does not move down, probe or fire the Torch).

Last thing which was very important is to turn of the merge circles option (either in Post Dialog or in the PP itself) since i got arc radius differs from start do end errors with any file.

I tried setting the Tolerances in the INI file <---- did not work.
Changing from incremental g91.1 to absolute coordinates did not work either.
Also tried the smoothing in Fusion, almost every tolerance setting in Fusion and Cam tolerance in the PP Dialog which did not work either.
until i turned off the merge circles option and it worked. 

I dont know if i am allowed to share the PP here for other People since docwelch created it but if its allowed i can post it if anyone has the same problems as i did.

Also sorry for the late reply i did some grassroots error searching for a few days only changing 1 setting at a time and looking for a difference in behaviour to fix the Arc radius error which took days and most of my freetime to finally find a solution ^^.

In case anyone is interested which changes i did to the PP here we go:
In the .cps file:

Line 27: tolerance = spatial(0.002, MM);
changed to:  tolerance = spatial(0.001, MM); 

---

Line 50:  MergeCircles: true --->>>  MergeCircles: false

---

Line 344:  writeBlock(mFormat.format(190), pFormat.format(tool.number));

(deleted so the Gcode does not specify the Material anymore)

---

Line 525: writeBlock(mFormat.format(3), $Format.format(2), sFormat.format(1)); //start the torch 
changed to:  writeBlock(mFormat.format(3), $Format.format(0), sFormat.format(1)); //start the torch

(the above corresponds to the M3 $2 S1 command which spins the spindle counterclockwise 
which did not work for my machine it did centerpunch however using the M3 $0 S1 command so i changed the 2 to 0 and everything worked fine)

---

If anyone has better ideas or suggestions feel free to share, changing these things in the PP finally got my machine working, cutting, and centerpunching.

I have just finished my first CNC machine so my solutions might not be the most optimal or even good but this is what got my machine working ^^
Any improvements are always welcome
regards



 

I'm also a fusion 360 user for a year now, and the merging circles thing was the biggest issue resolved since the radius bug was generated. I want to know if they have the trial or paid version to compare a cerntepunch code since I have problems and I have to fix it by editing the code and I want it to be automatic on the pp