The first thing you should do is see if you can find a relief or stl of the logo. Check etsy or stlfinder.com. 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:
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 ncviewer.com 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.