Hey again! Still learning and kinda stumped right now. I am using Fusion 360 to produce my tool path and CNC.js to run it. When I hit run in CNC.js the the first thing that happens is the Z wants to move straight down and try to go below the Z0 from where ever I jog the machine no matter where Z0 is. Would this be CNC.js or something in the gcode I did? Thanks for any help!
The post processor is a little weird. There is a newer one written. I’ll grab a link.
Here is the link to post processors:
https://cam.autodesk.com/posts/
The one made 10/23/17 deals with the Z-axis better. It also changes the way G2/g3 commands are dealt with. Also, in setup make sure your stock is the right size and in operations double check all of the heights.
i forgot to say, type tinyg into that search engine.
Tinyg? I’m using grbl@Colin_Kaminski
@Colin_Kaminski Found it! Thanks for the help!
@Nukpruf This forum has helped me a lot with Fusion issues. I was had editing every file for a long time before I figured out how to request a new post processor.
https://forums.autodesk.com/t5/fusion-360-computer-aided/bd-p/2070
Hey guys, great topic. This is universal for about all CAM softwares. Typically need a little tweaking to fit your machine perfect. I.e. G98, G64, G43, etc. some are used on some machines, and not recognized by others.
So both of you guys are using Fusion to draft and CAM, exporting GCODE directly from fusion?
@Brandon_Satterfield Hey Brandon. Not sure how to do the tweaking you mentioned (G98, G64, G43). And yes I use Fusion to draft, CAM and export, love it so far.
My workflow is paper>scan>Fusion>chilipepr
It is a long learning for fusion. I have about 8 months of daily drawing in now I still get surprises.
If you home your machine at. Z is the top of travel and use the G53 work space for your part the Fusion code runs perfectly without editing. Otherwise take the first G0 code and do something like this:
G0 X3.1 Y4.5
Z .2
Z .6
…
and change it to
G0
Z .2
X3.1 Y4.5
Z .6
This allows you to set the machine zero to the top of the part. I would also change the final Z code from G0 Z0 to G0 Z1 to retract the cutter off the part.
@Colin_Kaminski its very awesome that you are putting this kind of time in. I absolutely pays off when the machine becomes an easier to use tool than a pair of pliers.
I received this today as an export from a gentleman learning fusion and the related CAM:
G90 G94
G17
G21
G28 G91 Z0
G90
(2D Contour1)
M9
T1 M6
S10000 M3
G54
M9
Is this a typical header for stock fusion export?
I use various post processors in CAMBAM, they have never been such a mess. 
Yes, Here is one from the old TinyG post processor.
(1001)
(12 BULL NOSE)
(T1 D=12.7 CR=6.35 - ZMIN=-4.9 - BALL END MILL)
G0 G90 G94 G17
G21
G53 Z0.
(POCKET2)
M5
M9
T1
M3 S20000
G54
M9
G0 X-27.868 Y161.103
Z15.
Z2.
You can see it moves X before setting Z to retract height. Next is te new processor. I still haven’t figured out why it works better for setting Z correctly before it moves the XY axis. I have not yet learned all the codes in the header.
(1001)
(12 BULL NOSE)
(T1 D=12.7 CR=6.35 - ZMIN=-4.9 - BALL END MILL)
G0 G90 G94 G17
G21
G0 Z15.
(POCKET2)
M5
M9
T1
M3 S20000
G54
M9
G0 X-27.868 Y161.103
Z15.
Z2.