# (solved) Machine is not following program **URL:** \ **Category:** Elite Series (Masso & Redline) (Gen 1)\ **Created:** [May 20, 2026, 3:26am UTC](https://forum.onefinitycnc.com/t/solved-machine-is-not-following-program/38756 "2026-05-20T03:26:45Z")\ **Posts on this page:** 6\ **Page:** 1
**Author:** ![Chris\_Topher](https://avatars.discourse-cdn.com/v4/letter/c/7ea924/32.png) [@Chris\_Topher](https://forum.onefinitycnc.com/u/Chris_Topher)\ **Post date:** [May 20, 2026, 3:26am UTC](https://forum.onefinitycnc.com/t/solved-machine-is-not-following-program/38756/1 "2026-05-20T03:26:45Z")
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](https://us1.discourse-cdn.com/flex022/uploads/onefinitycnc/original/3X/7/f/7f28a5283ed5561688efba1f4bbb74b0345f8068.jpeg) ---
**Author:** ![L.M](https://avatars.discourse-cdn.com/v4/letter/l/a87d85/32.png) [@L.M](https://forum.onefinitycnc.com/u/L.M)\ **Post date:** [May 20, 2026, 10:54am UTC](https://forum.onefinitycnc.com/t/solved-machine-is-not-following-program/38756/2 "2026-05-20T10:54:51Z")
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](https://us1.discourse-cdn.com/flex022/uploads/onefinitycnc/original/3X/3/e/3ea500b3066cf0a5bcc3285b3b84f57efeb8d511.jpeg) ```auto (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](https://us1.discourse-cdn.com/flex022/uploads/onefinitycnc/original/3X/7/9/79cf871f71cd6d284e7d9cf6ae11dd32843c1028.jpeg) ```auto (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. ---
**Author:** ![Ken5](https://avatars.discourse-cdn.com/v4/letter/k/f0a364/32.png) [@Ken5](https://forum.onefinitycnc.com/u/Ken5)\ **Post date:** [May 20, 2026, 11:21am UTC](https://forum.onefinitycnc.com/t/solved-machine-is-not-following-program/38756/3 "2026-05-20T11:21:42Z")
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 ---
**Author:** ![Chris\_Topher](https://avatars.discourse-cdn.com/v4/letter/c/7ea924/32.png) [@Chris\_Topher](https://forum.onefinitycnc.com/u/Chris_Topher)\ **Post date:** [May 20, 2026, 2:06pm UTC](https://forum.onefinitycnc.com/t/solved-machine-is-not-following-program/38756/4 "2026-05-20T14:06:12Z")
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 ---
**Author:** ![MikeXYZ](https://sea2.discourse-cdn.com/flex022/user_avatar/forum.onefinitycnc.com/mikexyz/32/32034_2.png) [@MikeXYZ](https://forum.onefinitycnc.com/u/MikeXYZ)\ **Post date:** [May 20, 2026, 3:20pm UTC](https://forum.onefinitycnc.com/t/solved-machine-is-not-following-program/38756/5 "2026-05-20T15:20:43Z")
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. ---
**Author:** ![Chris\_Topher](https://avatars.discourse-cdn.com/v4/letter/c/7ea924/32.png) [@Chris\_Topher](https://forum.onefinitycnc.com/u/Chris_Topher)\ **Post date:** [May 20, 2026, 5:42pm UTC](https://forum.onefinitycnc.com/t/solved-machine-is-not-following-program/38756/6 "2026-05-20T17:42:28Z")
Solved, I changed the cutter comp from wear to in computer, and removed the sequence numbers, and its running as it should now.