Facing Pass SO3 and Fusion 360 -- bit not making contact with stock

Usually such problems are a disagreement in where / how the Z-axis origin is declared — maybe something here will help?


  1. From your photo, it looks like you set your stock as the same thickness as the finished stock. If I am seeing that correctly, your gcode output will not remove any material. Meaning you need to set your stock thicker OR your finish part, thinner. There are other ways to lie to the machine, for a quick fix, but I’d rather not discuss those options here (yet) (It;s hard to see the 1mm)

  2. Where did you set your Z0 (At the top of the material OR 1mm below)?

1 Like

I think I set the stock thicker than the work piece. I set the WCS origin at the corner of the work piece.

I set my Z origin at the top of the MDF (jogged the bit down to make contact with the MDF and zeroed all in Carbide Motion).

It is cutting WAY more than 1mm above the top of the work piece.

All I see at that link is a single page showing the F360 post process panel. Is there something else?

If everything is set correctly (XYZ0), then go into your F360 Facing operation and look at the depths tab. It should start from the Stock Top to the Bottom Model Top (See photo)

Or you can email me the F360 file and I can look at it, OR you can share the folder.


There’s a bit more at: Shapeoko CNC Router, Rigid, Accurate, Reliable, and Affordable

Available under an annual license w/ pricing ranging from zero to $300 to $1200 annually.[18] Fusion 360 | 3D CAD, CAM, CAE, & PCB Cloud-Based Software | Autodesk Knowledgebase article on activating startup or educational licensing[19]
CAM tutorial[20]

There is now a Carbide3D post-processor: Fusion 360 Help [21] Notes on post-processor for associated CAM: Shapeoko CNC Router, Rigid, Accurate, Reliable, and Affordable https://forums.autodesk.com/autodesk/attachments/autodesk/2070/3456/1/carbide3d.cps [22]


Fusion 360 Help [23]

Autodesk Fusion 360 CAM Post-processor for ShapeOKO – Restricted Ayerspace [24]

shapeoko post processor.zip[25]
GitHub - Strooom/GRBL-Post-Processor: Post Processor for Autodesk Fusion360, delivering GCODE output optimized for GRBL compatible CNC or Lathe [26] — free / opensource / documented Post-Processor which translates RPM values into dial-settings for Dewalt and Makita trim routers, and will alert you and recommend solutions for some errors in a design. Modified version: C3D-SO3-DEWALT.cps.zip[27]

Post Library for Autodesk Fusion 360 | Autodesk Fusion 360 [28]

Note that some users have found it necessary to increase the precision for metric files so as to avoid Invalid Gcode Error 33: GRBL ERROR: Invalid gcode ID:33 - #10 by jeff5280 with Carbide Motion 4 and Grbl 1.1, there is a setting which may need to be changed to avoid a similar error: Fusion 360 and GRBL errors - #9 by patofoto

Free license available to hobbyists and startups making less than $100,000 annually (must be renewed each year, details: Autodesk - Legal Notices & Trademarks - Autodesk Web Services Entitlements ): How to register for a start-up, personal, or student license for Fusion

Engrave/V-carving added as a feature.[29][30]

Adding tabs when cutting 2D feature: Shapeoko CNC Router, Rigid, Accurate, Reliable, and Affordable

Job setup

Step and repeat is termed a “Pattern”.[31]

Notes on scaling of SVG files: How To Fusion 360: Simple Wine Rack - #9 by markmoran

Discussion of limitations: Shapeoko CNC Router, Rigid, Accurate, Reliable, and Affordable

Has problems when model is defined in Imperial and CAM is done in metric.[32] Metric should be used to avoid Grbl Invald G-code #33 error.[33]

Criticism on Reddit: Reddit - Dive into anything

FEA and interference analysis (complex FEA can be performed via AutoDesk’s servers for an additional cost). Uses a joint based system to limit degrees of freedom and a top down (as opposed to bottom up) assembly system.[34]

Cribbage board: Fusion

Fusion 360 for the Nomad - #21 by UnionNine

Useful plugins [35][36]:
https://github.com/hanskellner/Fusion360Image2Surface46 — Fusion360 plugin for converting an image (height map) to a surface. Has a neat example with a penny.
https://github.com/hanskellner/Fusion360SoftJaws22 — Creates soft jaws automatically.
GitHub - tapnair/NESTER: Simple script to lay parts out flat in Fusion 360 — Flattens a 3D design specifically for use with a CNC router…
GitHub - CrypticRage/BossJoints: This is an addon for Autodesk Fusion 360 that assists in drawing different types of joint geometry. — for CNC joints
GitHub - benbreen/Cycloidal: Cycloidal Gear Generator for Fusion 360 — for generating gears and pinions.
GitHub - visualapproach/WeirdGears: Fusion 360 python Add in to make non circular planet gears — non-round gears

https://www.7thdensity.com/single-post/2017/04/19/Two-sided-machining-with-Fusion-360 [37]

Except that you are dimensioned in inches, I am seeing what you are seeing in the heights tab.

I’ll take you up on the offer to look at the file. I am out the door to work right now and F360 is telling me there is a “temporary outage”…

The two things I would note are:

  1. set the stock for this as relative size box, not fixed size box. The top offset is then the material to remove.
  2. In the setup tab, be sure you selected the zero properly. Z=0 wants to be the top surface of the stock (stock box point option)so you can touch off the tool to it. You do not show this (setup tab), but it is a common issue.

If you care about the finished thickness of the waste board, you would set fixed size stock and set the zero to the bottom of the stock, but zeroing the tool would be more difficult.

When I did my facing I kept it simple. I created a model of the wasteboard I wanted to face then in CAM I just created a facing operation with a depth of 0.5 mm. That’s it. When I got to the Shapeoko I just zeroed my bit height on the high point of the wasteboard then set the x and y to the proper corner or center of the wasteboard depending on where you set it in CAM. Take a pencil and lightly mark the top of the wasteboard randomly. I just run long squiggles all over the entire surface. Run the cycle once and see if you removed all of your pencil marks. If not then re-zero your z height to the surface you just hit then run it again. Repeat until all of your pencil marks are gone then you know you have flattened the entire surface.

1 Like

FWIW, there’re files for doing some of this in Carbide Create here: Wasteboard Plans with threads

THANK YOU! That did it.

New problem. Its cutting deeper when moving in the in the +x direction than when moving in the -x direction.

That suggests to me a loose v wheel. Top right maybe?
Bottom left, I mean. Mine’s upside down.


I am trying to figure out how this would cause the observed failure? Is it that the z-carriage rotates in the x-z plane when being driven in the x-direction?

How could I tell if a wheel was loose? I cannot feel any play in the carriage when I twist it, nor do either of the wheels turn freely – that is, if I stick my fingers in there and rotate either wheel the carriage rises and falls and the wheels do not seem to slip.

I am done playing with it for the night. I’ll try running the facing passes in just one direction (conventional milling) and/or in the +/- y direction.

1 Like

Your router isn’t exactly perpendicular. It could be leaning slightly to the left or right and/or to the front or back. It’s hard to tell but what I’m seeing it looks like the router is leaning forward a bit. The front edge of the cut looks like it’s lower than the back side of the prior cut. Someone else suggested that this could be a loose v wheel and that’s a good place to start. You could also double check to make sure your router is really sitting in the mount straight.



There is some barrel distortion in the image. I’d be reluctant to say this is the case across the board (there is some warp and bow in the piece) , but from what I can see with my face down on the bench the walls of each of the deeper cuts are the same height back and front – not saw toothed.

I’ll check that the router is square and rigidly seated.

I think @Rick is right.
There is a good tune up video here:

Especially in your case watch at 5:09 “Squaring your spindle”.

1 Like

If the router is leaning left or right then you’ll get that wave pattern since the left or right side of the bit is cutting deeper. The bit is round so that ends up being a wave pattern. Winston covers that in the tuning video that someone else posted.

1 Like

Thanks all.

:slight_smile: I am a fan of Winston Moy’s channel too. In fact, it was watching the video that Jerry Gray posted that has me making a supplemental waste board in the first place. I am going to cut both sides of some tight-tolerance pieces, and I need something flatter and more square to the cutter than the bits of MDO scrap I’ve been using as spoiler board.

By “scalloped” cuts for a spindle rotated about the y-axis (tilted left/right) I understood Winston to mean depressions running perpendicular to the direction of the cut – but I admit that I was puzzled by that bit of the video.

It really doesn’t photograph well, but the cuts alternate deep/shallow. Almost 1 mm deeper on the +x cuts than on the -x cuts. The walls of the deeper cuts are the same height front and back. It is not sawtoothed. I put some 0.7mm pencil leads in and across one of the deeper cuts and pulled out my cheap macro lens. It still doesn’t show up well).

I am using a Magnate bottom clearing router bit. Its only 7/8 of an inch across, so it is not as sensitive a measurement as Winston’s improvement-on-a-coat-hanger-tool, but pushing the bit down onto a flat and parallel piece of plywood laid flat on the base of the S03 I don’t see any gaps under the cutter in either the x- or y- direction.

Giving it a little more thought, I’d guess that running this bit with the rotation is causing it to climb out of the cut – which makes me wonder what part of the S03 is deflecting upwards when this happens?

I’ll try running the passes in one direction and report back for further advice and correction in the morning…

1 Like

Things to check:

  • Z-axis belt tension
  • V-wheel tension
  • pulley set screws
  • springs (try a test cut removing one)
  • depth per pass too great — you should only be removing a couple of thousandths at a time (if that)

Usually you can push / pull on the router collet and see where things shift about — sometimes you can hear a “click”.

Arguably, this path would be best w/ a consistent direction — might want to hand-code it to enforce that.

Next up on the Carbide 3D channel — tramming your wasteboard in alternating directions and paths so that it doesn’t develop a grain (anyone else do that when cutting their grass?)

1 Like

Thats funny.
I was just mowing yesterday.
I always think about “milling” the grass.
Climb mowing, or conventional?

1 Like

Decided to make some chips before going in to work this morning.

F360 lets you set up both-ways, conventional, or climb. For facing it defaults to both ways.

I got what I was after with conventional milling.

There was significant bow towards the middle of the piece, so it took three passes to clean up the canyons left by the first attempt. I ran the second and third passes in the y-direction after which I noticed some some very faint tool marks. Running my finger over the surface I could just feel a little ridge on the left side of every pass – so my spindle is rotated slightly out of square around the y-axis. Not enough to affect my next couple of projects, but I will fix it when I have time.

Thanks everyone for the help and advice.

1 Like