Introduction

I've always been intrigued by the possibility of making circuit boards at home. So when I got a CNC machine, one of the first things I wanted to try was fabricating custom-made circuit boards. I focused on creating a reliable process that can be easily followed and is almost guaranteed to produce same result over and over again.

Despite it being a DIY process, I was still interested in creating boards that are somewhat comparable to commercial ones, which meant having a soldermask, and (to some extent) silk screen. At the same time, I was not under the illusion that it will ever match what you can get from many online PCB fabrication places, but it's sufficient for most hobby applications.

This process shown here covers producing a double sided circuit board using Makera's Carvera CNC machine. It's desktop-size machine with work area of 36 * 24 cm, 200W spindle, accuracy in the range of <0.01mm and integrated 2.5W laser module. However, to some extent, this process can likely be applied to just about any CNC machine.

The process covers:

Drawing and exporting a PCB in KiCAD
Creating routing job using FlatCAM
Preparing a board cutout and align holes using MakeraCAM
Routing
Applying solder mask
Removing solder mask from pads
Flipping and aligning the board
Applying silk screen
Drilling holes for through-hole components

Finally, I'd like to point out that there's not a lot of novelty in this process, but it's a collection of different techniques made with inspiration from others seen online. There will be credits through the guide to different sources.

Limitations

So far, this process has been reliably test out on components as detailed as LQFP48/64 package. This means package size of 10x10mm and pads of ~1.2x0.25mm, spaced 0.5mm apart.

(source: https://www.ti.com/lit/ds/spms376e/spms376e.pdf, p.1404)

This was also used as an inspiration for design rules when making a PCB. Namely, minimum trace size of 0.2mm and clearance of 0.2mm.

Here's few of the examples made with this process:

This rest of this guide is going to follow a whole new board from scratch to something comparable to the examples above. See "Build instructions" section below.

Build Instructions

Collapse

1
KiCAD design + export
When laying out a board in KiCAD, there's few tips to follow:
- Minimum track width: 0.2mm
- Minimum track clearance: 0.2mm
- (optional) Don't do clearance to the board edge (source: https://forum.kicad.info/t/zone-to-board-edge-clearance/45386/4)
- Place symmetrical align holes, for example a hole in every corner, exactly 3mm from the edge
- Place board "Grid origin" and "Drill/Place File origin" points in the bottom left corner of the board
- Take special care of through hole components! This PCB doesn't have plated holes and so the component needs to be soldered from both sides in order to link top and bottom layer. KiCAD will by default link signals or ground planes using a through hole component, in the same way it does with a via. However, some components might not make the top side available.
For through-hole component that cover the soldering point on the top layer, it might be a good idea to route a "backup" track on the back layer, just in case it's not possible to solder them from the top, or only route on the back layer where you're sure to get good contact.

Finally, before exporting, make sure the check

Export

To export the files, navigate in KiCAD to Files -> Fabrication output -> Gerbers (.gbr) ...
- Set output directory, e.g. "CAM"
- Include layers: all copper, silk, mask and edge cuts
- Under "General options", select "Use drill/place file origin"
- Before export, it's a good idea to run design-rule check. This will provide feedback on any unconnected tracks, overlapping silkscreen etc that should be fixed
- Finally, press "Plot" to export the files
- Then, press "Generate Drill Files" to export drill patters and sizes
  In the new window, make sure "Drill File Format" is "Excellon" and "Drill origin" is "Drill/place file origin"
  Finally, press "Generate Drill File"
- Close both dialogs
2
FlatCAM
Isolation Routing
To process exported files into a CNC job, we'll use FlatCAM.
- Start by importing F.CU layer
- Double-click the layer and and select "Isolation Routing"
- In the tools table, we'll set tool diameter to 0.19mm. This has to be lower than the "Minimum track clearance" setting in KiCAD to ensure correct routing. As a side note, I'm using 0.2mm V-bit for isolation routing. So the correct setting here would be 0.24mm instead. So in reality, all the pads and tracks will be 0.05mm undersized. I have tried this step with bit diameter as low as 0.1536mm for a 0.2mm bit, and the results were still satisfying.
- To generate the CNC object from geometry, set V-Tip diameter 0.15mm for cutting depth of -0.0746mm.
Settings

Copper clearing
Usually, it's enough to just do isolation routing, but sometimes, there's the need for clearing copper areas. FlatCAM has NCC feature for that.
This can be used to generate geometry and a following CNC job.