Interested in CNC Wisdom

Hi Everyone,

I’m embarking on a project with an ambitious timeline. Right now I’ve got the laser module carving a path into oak plywood that I can cut out with my scroll saw and plunge router (pattern involves a circle and will need to be produced twice for desired thickness so I wanted exact lines) (

I am thinking of using the CNC module carve out the words at the top of the linked image patch (and may change the words at the bottom) within an arc-shaped pocket.

This won’t need to be terribly deep, but deep enough the letters stand out. After looking into some threads/basics, I’m a little daunted getting started with the CNC.

Among my chief concerns is getting it to carve out exactly where I need within the shape. I’ve fought with the laser lately to burn exactly where I want and I’m worried about the same with the CNC.

Also, the concept of generating tool paths and switching bits is not something I’ve done before and it feels challenging (maybe its super easy, but I don’t feel that way at the moment).

I can easily produce the shape and words in Fusion360 to make a 3D model/relief, are there any tips, hints, tricks, threads you all might be willing to share for a crash course in trying to make this happen?

I know the most likely response, which I accept the full appropriateness of, might be “just google it.”

I’ve searched out a few threads I’m planning to review, but any tips, tricks, lessons, links to useful threads etc. would be most appreciated.

Thank you!

The first thing you should do is see if you can find a relief or stl of the logo. Check etsy or May have to pay but trust me, it probably will be worth it. Failing that find an svg (vector) version of the logo.
If that’s not available, is there a version without gradients/shadows/textures?
Because you’re going to need to go in and do some editing in an image program that allows you to create layers and separate the different elements. It’s a lot easier if the selection tool can easily choose elements.

I’m not sure if you’re trying to actually cut out the individual pieces and assemble them, or if you’re trying to carve it out of a single piece of wood with varying heights. The following information is for the latter.

Here’s an example of a logo I’m currently using for a tap handle:

I went in and separated it into the different layers that I was going to have at different heights.
I duplicated the main image once for each color and then deleted everything but one color on each layer. Then I exported each layer separately as a png file, and then used Inkscape to trace the bitmap and save each as a simple svg:
Screen Shot 2021-05-16 at 9.43.14 PM

Then it’s simply a matter of importing the svg’s into Fusion and selecting and extruding the elements to the desired heights/levels: (one word of advice: when you’re doing depths in cnc, they turn out a lot deeper than you’d think. On this patch (80mm dia) most differences in level are just 1mm and over-all for the 5 levels it’s just 5mm)

Then you go into the manufacture section of Fusion in ‘setup’ and tell it where you want the work origin to be. Generally you’ll either want A)bottom left and top of stock or B)center and top of the stock. (On cnc you’re working top down, opposite of 3d printing) Remember which one you choose and set the work origin appropriately on your SM when you start. Then enter the correct info for stock size (watch out for it trying to round up automatically)
Then select the appropriate paths for the bits you have/plan to use. If you’ve only got flat surfaces you only want (need) to use flat end mills.
Generally I start with 1/4" bit and 3D pocket clearing tool path for main clearing with 1mm stock to leave.
Then 3.175mm and pocket with .5mm stock to leave.
And then pocket and pencil (or parallel with both directions passes) for my finishing pass with my smallest bit I’m going to use (on the patch I went with .8mm).

The key settings for any path are:
Geometry - what area you want it to mill
Heights - Top height (where it will start to cut.) Bottom height (the lowest level it will cut)
Step-down - .5mm is generally safe to plan on, 1mm on some softer woods.
Rest-machining - Can be off on first tool path, after that it tells Fusion to ignore everything
that’s been previously milled, so you’re not just milling air.

Then fusion will figure out exactly where and how to do everything for you and account for size of bits.
Once you like the look of all your toolpaths, select them all and run a simulation and see how it looks and if there are any errors that you need to adjust for.
With SM you’ll need to export each tool as it’s own tool path. (Multiple passes with same size bit can be exported together. Export each using ‘post process’ and make sure to end the name as .cnc
Use to see if the gcode is doing what you think it should be.
Here’s some more info on tool changes and cnc in general:
Some info on cnc tool changes and combo cnc/laser projects

Before you start a job with new gcode running on your SM, and after having set the work origin, raise the head and bit far above anything it can run into and run boundary. If everything looks okay as far as that, then it’s not a bad idea to set your z-origin far above your work piece and start the job and watch what it does in the air. Then if that looks okay set your z-height to where it should be and start the job. Anytime you’re doing any of this it’s a good idea to make sure you have the power button within easy reach, if not your hand on it.

Hopefully that’s the kind of info you were looking for.
CNC can seem like a really steep learning curve at first. It’s definitely the hardest thing to do on SM by a mile. A lot of that is just learning Fusion and a few different things to get your head around. Lots of new terms and remembering it’s a subtractive process - you’re removing material from an existing item in contrast to 3d printing which is additive.



SDJ, I skimmed your post and I have to say thank you so so much for such an in depth reply! I’ll be back soon to pour over this in detail.

To answer the question you asked, all I want to engrave are the words at the top and bottom. I used the laser module to cut the outline of the frame as shown below. The outermost line I’ll cut with a scroll saw, the next line in will be a painted accent, and the inner circle I’ll cut out with a router and circle jig (to make an infinity mirror).

While I could laser engrave the words at the top and bottom, I would really love to CNC them out (in an arc-shaped recession between the circle’s arc and the inner of the 2 outer lines).

So those are my plans and you may very well have come to my rescue. Thank you again, I’ll let you know if I have any questions once I can really absorb your reply.

For scale reference the board below the tape is 13 inches (X Axis) by 15 inches (Y Axis) (intentionally larger than the Snapmaker laser platform on all edges).


Okay I’ve read your reply in full and most of it seems pretty straight forward. Great, simple directions!

If I am carving out letters, lets say B, R, D, O (anything with a center), does that center need to be a separate tool path?

So my Fusion layers and tool paths will first cut the outside around all the letters and the overall indentation I want, then a separate layer to cut each letter hole to the correct depth?

Based on that simple summary is there anything I’m missing?

If you’re using engraving than you need to select each path separately.
If you’re doing any other kind of tool path Fusion will automatically remove what needs to be removed and leave what’s supposed to stay within your selected areas (By default it will do everything of your model)
You can choose your whole piece or various sections.
I find it handy to make what I call ‘ghost objects’ sometimes. Shapes that match the area I want to carve within. If you turn off visibility before going into manufacture they’ll be ignored, but you can choose them to define boundaries.(or parts to ignore). Just be careful they don’t change the size of your stock unexpectedly.
You can also use sketches (your imported svg’s and use for selections).
If I choose this edge under geometry it will only carve what’s inside it (and within the heights I’ve chosen under the heights tab) and that it can carve with the selected size of bit.

If I select inner and outer ring it will only machine between the two.

I can just select the face of the wings and it will only carve those:

By changing/adjusting tool containment I can select whether it stay inside those boundaries or will include a selected distance outside.



This is a great resource for us newbies, thank you so much. I’m currently mustering the courage to try my first CNC project too, and this breaks down the steps so clearly that it really doesn’t even seem intimidating.

In case you were wondering, here are the final results of my example:



You are most skilled user I’ve seen. Thank you for sharing these works.


Thank you for the kind words @Edwin
It’s a very capable machine as long as you understand its limits and capabilities.

I would love to see what I could do with the Rotary Module but at the present it’s beyond my budget. Still making up for lost work and wages from Covid.



@sdj544 I saw you linked this thread recently and realized I never posted the final result:


Nice work!
Turned out beautifully!


1 Like