Introduction
Welcome back to Part 2 of our
PCB Milling Master Class. In
Part 1, we covered why milling your own boards is the ultimate prototyping hack. Now, it’s time to actually design one.
You might be thinking, "I already know how to design PCBs. I’ll just take my existing file and mill it."
Stop right there.
If you try to mill a board designed for a professional fab house (like JLCPCB or PCBWay), you are going to fail. Why? Because lasers and chemical baths have almost zero physical width. A CNC bit, however, has a physical tip. If your traces are too close together, your V-bit won't pass between them—it will plow right through them, erasing your circuit.
Today, we are using EasyEDA to design a board specifically for the physical limitations of a CNC mill.
Why EasyEDA?
For this series, we chose EasyEDA because it runs in your browser, is completely free, and has a massive library of components. However, these concepts apply equally to KiCad, Eagle, or Altium.
The Golden Rule: Clearance is King
When ordering a pro board, you can get away with 6 mil (0.15mm) clearance between traces. On a home CNC, you need Breathing Room.
Your isolation bit (usually a V-bit) needs space to travel. If you put two copper pads 0.1mm apart, but your V-bit tip cuts a 0.2mm path, it will connect those two pads together. Short circuit.
Recommended CNC Design Rules:
- Clearance (The most important setting): Set this to 0.3mm or 0.4mm (approx 12-16 mil). This ensures a standard 30-degree V-bit can pass between traces without destroying them.
- Track Width: Thicker is better. I recommend a minimum of 0.5mm (20 mil). Thin traces peel off easily during soldering if you aren't careful. If you have the space, go with 1.0mm tracks. They are robust and carry current well.
Adjusting the default clearance to 0.4mm in Design Manager.
Setting Up EasyEDA for CNC
- Open your PCB Layout.
- Go to Tools > Design Manager > Design Rules.
- Change the Default Clearance to
0.4mm.
- Change the Default Track Width to
0.5mm.
Now, as you route your board, the software will physically prevent you from putting traces too close together. If you use the "Auto-Router" (we won't judge), these rules will force it to space things out properly for your machine.
The "Via" Problem
In a pro board, a "via" (the hole that connects the top layer to the bottom layer) is plated with metal. Electricity flows through it magically. Your home board is just a piece of fiberglass. The hole is not conductive.
To make a via work at home, you have to stick a wire through it and solder it on both sides.
- Design Tip: Do NOT place vias underneath chips or sockets. You won't be able to reach the top side to solder them. Move all vias out into open space where you can easily reach them with a soldering iron.
- The Header Trick: We will cover this in detail in Part 5, but for now, make your via holes 0.8mm or 1.0mm. This allows you to use a standard Arduino header pin as a "rivet" to connect the layers.
The "Through-Hole" Problem
Since the holes in your homemade board aren't plated, the solder won't wick through from the bottom to the top.
- Top-Layer Traces: If you have a trace connecting to a component on the Top Layer, you must be able to solder that pin on the top side.
- The Issue: Plastic connectors and IC sockets sit flush against the board, hiding the pads.
- The Fix: Design your board so that connectors and sockets mostly connect on the Bottom Layer. If you must connect on top, be prepared to mount the component slightly raised off the board so you can get your soldering iron tip in there.
Exporting for the Mill
Once your board passes the DRC (Design Rule Check) with no errors, it's time to export. FlatCAM (the software we will use in Part 3) needs standard Gerber Files.
- In EasyEDA, go to File > Export > Gerber.
- Download the ZIP file.
- Unzip it. You will see many files, but for milling, we only care about:
Gerber_TopLayer.GTL (Top Copper)Gerber_BottomLayer.GBL (Bottom Copper)Gerber_BoardOutline.GKO (The profile cut)Drill_PTH_Through.DRL (The holes)
What's Next?
You now have a set of files designed specifically for the capabilities of your machine. But your CNC doesn't speak "Gerber"—it speaks G-Code.
In Part 3, we enter the beast: FlatCAM. We will show you how to import these files, generate the isolation toolpaths, and the critical step of creating Alignment Holes so your double-sided board lines up perfectly when you flip it over.
Get your V-bits ready. We start cutting in the next episode.