(solved) Machine is not following program

Elite Series (Masso & Redline) (Gen 1)
1

I have the gen 1 elite journeyman with masso g3 controller. I recently got the machine setup and trammed. Even had successfully made and used a facing program for my spoil boards on fusion360 using the masso post.

Now Im trying to run my first part and the machine is going far off course from the g-code in the program, dispite the work coordinates being correct. (this is what im showing in the photo)

I tried using a g57 instead of g54, but no difference. I used MDI and entered in g57x0y0g0 and the tool goes right to the correr of the part as it should. But after I click start on the program the z seems correct but the xy just start heading off the part. And it also shows in the grafx representation that the tool is going way off. I’m very familiar with CNC machines but I’m stumped with what could be the issue here.

20260519_192154
20260519_1921541884×4080 1.57 MB

2

Is it possible it’s due to where you’ve defined the WCS in your CAM software?

I ask because I notice in your gCode the first X move is positive where I’d expect it to be negative if you were working off the upper right hand corner of your piece.

I threw together a quick sample file in Fusion to demonstrate what I’m talking about:

If WCS in Fusion Manufacture CAM is set to lower left (where I generally start) then the first X move is positive whereas if I set it to the upper right then the first X move is negative:

LOWER LEFT WCS

Screenshot 2026-05-20 at 06.46.42
Screenshot 2026-05-20 at 06.46.423156×2268 452 KB

(RTCNC FUSION POST PROCESSOR V2.0)
(LOWERLEFTWCS)
(MACHINE)
(  VENDOR: ONEFINITY)
(  MODEL: ELITE JOURNEYMAN)
(T11 D=6.35 CR=0 - ZMIN=8.5 - FLAT END MILL)
G90G17
G21
G53G0Z0

(POCKET1)
T11
M6
S12000M3
G17G90
G54
G0X52.949Y52.637
Z33
G0Z22.668
G1X52.936Y52.629Z22.53F333.3
X52.897Y52.607Z22.399
X52.835Y52.57Z22.28

UPPER RIGHT WCS

Screenshot 2026-05-20 at 06.46.57
Screenshot 2026-05-20 at 06.46.573108×2182 443 KB

(RTCNC FUSION POST PROCESSOR V2.0)
(UPPERRIGHTWCS)
(MACHINE)
(  VENDOR: ONEFINITY)
(  MODEL: ELITE JOURNEYMAN)
(T11 D=6.35 CR=0 - ZMIN=8.5 - FLAT END MILL)
G90G17
G21
G53G0Z0

(POCKET1 (2))
T11
M6
S12000M3
G17G90
G54
G0X-47.051Y-47.363
Z33
G0Z22.668
G1X-47.064Y-47.371Z22.53F333.3
X-47.103Y-47.393Z22.399
X-47.165Y-47.43Z22.28

FWIW, I’m trying to divine a lot from the screen shot and the code, but in the past when I’ve had odd movements it was generally because I didn’t set the WCS in CAM properly. In my case Fusion defaults to the center of the piece, so I’ve had to build moving the WCS into my workflow.

3

I don’t use Fusion but I know when ever I’ve had a machine take off in an unexpected direction it was one of 3 things

  1. Work origin was not set correctly to work piece (0,0)
  2. There was something created off screen in the software so not visible unless you zoomed out
  3. Wrong post processor- MM or Inch or wrong machine type
4

I am using lower left corner, And it shows that I setup the x0y0 correctly when I call g57x0y0g0 in MDI. Someone mentioned in the facebook fourm that I should not be using incremental arc interpolation, so im going to try and make that absolute arcs and see if that solves it

5

Perhaps try posting a very simple G-code, like a simple square with no curves. This would help rule out any weird behavior caused by curves.

The program would be short enough for you to post the whole thing here, and we can view the commands line by line.

6

Solved, I changed the cutter comp from wear to in computer, and removed the sequence numbers, and its running as it should now.