My first CNC sucked - that's OK - how do I improve?

My first attempt at CNC milling totally sucked - but that’s what I expected - and that’s OK.
How do I improve?
First, can I do better with a choice of material? This is cedar. Is this too soft? What choices for high resolution / high detail would work better?
This first image shows typography - I expected this to totally blow and indeed it does. Clearly the bit is too big for the type face / size. The bit used for this project is a dual flute flat nose. Given the flat nose, there’s no way to cut with detail smaller than the head. OK - I am not allowed to post two images in one message so this first image is not shown.
Can the bit be changed in mid-job? If so, what is the best practice for this?
This second image is derived from a high resolution image of Abraham Lincoln. Again, the results are horrid - but that’s OK - the point is to learn. The bit used is the same flat head dual flute. work speed is the default (300). Step down is 1 mm. Density is 20. The Luban tool-tip says 10 is the max, but 20 is allowed.
To produce the highest resolution possible, should I be using different bits? Multiple bits? Different settings?
Thank you.

Here is the typography.

I’m also pretty new to CNC, but here are a few things I’ve pieced together since getting my SM2.

  • The bits that SM sells are very delicate, and perhaps not the best for removing large amounts of hard material. I bought some larger bits (and larger diameter collet) to handle the aggressive clearing. They’re fine for precise 2D cuts in acrylic, engraving etc.
  • If you use CAM software like Fusion 360, you can define multiple steps for your work. I haven’t tried using Luban beyond the initial out-of-the-box test of cutting the acrylic phone stand as I was already comfortable working with Fusion and it felt like I had more control over the process. There are plugins available for Fusion that allow you to create 3D models from images.
  • E.g. rough out the stock using “3D Adaptive Clearing” with a larger tool, leave plenty of “meat” by setting the axial and radial “stock to leave” at about 1mm or more if you’re getting too much tear-out.
  • Create “derived” tool paths using more delicate tools with finer detail contour tool paths. Ensure “REST Machining” is enabled so that the derived tool paths know what stock has already been removed, and what needs to be cut.
  • Reduce the step-down, plunge rate and cutting feed-rates until you’re confident the machine isn’t struggling to cut. Lots of shallow passes will get better results than one or two aggressive passes.
  • For round edges or more organic shapes, get yourself some good ball mill bits. Fine ball mill bits (.5mm diameter or less) produce surprisingly fine detail carvings, and with a 6mm shaft they are sturdy enough to remove a fair bit of material very quickly.

In other words, CNC machining of sculptures or bas reliefs on SM2 is a progressive process - you start with aggressive tools and toolpaths, then proceed to increasingly higher precision, finer detail tools and passes until you reach the desired surface finish.

CNC speed and feed calculators used for bigger machines tend to be a bit optimistic for the SM2. If you watch and listen as the machine runs you should be able to see if the tool is deflecting too much or chattering on the stock, and hear if it is struggling to make the cut. Dial your step-down and speeds down until you find the sweet spot. (You can sort of do this by adjusting work speed from the touchscreen while it’s working, but this is not ideal as it slows everything down, not just the feed rate or plunge rate).

I’ve also found it useful to stop and think about speeds and feeds in units per second rather than units per minute. 1 metre per minute doesn’t sound like much, but 1.6cm per second is a pretty fast cutting rate. I’ve found this approach particularly useful when thinking about plunge rates - if I were drilling a hole by hand would it go that fast?

Keep at it. Mastering the process is a rewarding feeling!


SimonF is spot on. If you’re trying to get 3D resolution, ball end mills are the way to go. If you’re just clearing material out, flat end mills should be used. As far as your feeds and speeds go, that’ll come with time and experience. I’ve spent a fair amount of time with scraps of whatever material I want to work on - just getting it dialed.

Regarding tool changes, Luban isn’t a good option. Honestly, Luban isn’t a good option for most SM operations. I always use Fusion 360 for my CNC paths. You can do tool changes one of two ways. Either program the tool change into the gcode, or (and this is the easier method I use) simply use one gcode file for the roughing passes, and then create another for the finishing passes. This way, you can change tools and only have to change the Z value for your work home (to adjust to the new tool).

I usually start with a 3.175mm flat end mill to remove as much material as possible. I’ll then step it down either with a ball end or a flat end - depending on if I’m going 2D or 3D. For cedar wood, I would recommend using a 4 flute corn flat end mill. It will give you a much better finish than a 2 flute. I’ve got a range from 3.175 to 0.5mm diameter bits. It’s always good to have options to step down to. Naturally, the smaller bits will take longer, but they’ll give you much better resolution.