* SYSTEM.NOTICE: Affiliate links support continued laboratory research.
By Day 31, you built a fully functional Smart Home Hub. It works brilliantly. The code is optimized, the network stack is robust, and the physics are sound. But look at it. It is a mess of jumper wires, dangling resistors, and a breadboard that could disconnect if you simply sneeze. This is not a product. It is a prototype.
Today, we cross the most significant chasm in electronics engineering: The transition from Breadboard to Printed Circuit Board (PCB). We will take the exact circuit from Day 31 and turn it into a permanent, compact, and reliable manufacturing file that you can order from a factory.
Why do we design PCBs? Itās not just about aesthetics.
The Tool of Choice: EasyEDA We choose EasyEDA for this guide because it is:
A PCB Design has two distinct files: the Schematic (Logic) and the Layout (Physical). You must start with the Schematic.
Open EasyEDA Editor. We need to replicate our Day 31 Smart Home Hub. Search for these specific LCSC Part Numbers or generic terms:
Critical Engineering Rule:
Net Labels: Keeps the schematic clean.
NetPorts: Dedicated VCC and GND symbols.
Labels: SDA, SCL, RELAY_SIG.
Why? This keeps the schematic readable. If you connect a label SDA to the OLED and SDA to the ESP8266, the software knows they are connected.
In a schematic, a resistor is a squiggly line. In the real world, it can be a tiny 1mm chip (0402) or a big 5-watt ceramic block.
The Symbol: The logical representation (Pin 1 to Pin 2).
The Footprint: The physical land pattern (Copper pads on the board). Critical: EasyEDA lets you pick a generic āResistorā symbol. If you donāt assign a Footprint, you canāt build the board.
Best Practice: Always select parts from the āLCSC Libraryā. These come with a Symbol, a Footprint, AND a 3D Model linked together.
Verification: Press Space on a component to rotate it. Double-click to check its āPackageā attribute. If it says None or AXIAL-0.4 when you wanted 0805, fix it now.
When you finish drawing, the software generates a Netlist.
This is a text file that lists every connection:
NodeMCU.Pin.D1 <--> OLED.Pin.SCL
NodeMCU.Pin.D2 <--> OLED.Pin.SDA
Run the ERC (Electrical Rules Check):
Before moving to layout, click Design -> Check DRC/ERC.
It catches errors like:
Floating Inputs: Pins that go nowhere.
Short Circuits: VCC touching GND.
Rule: 0 Errors, 0 Warnings. Do not ignore warnings.
Click āConvert Project to PCBā. You will see a black screen with a jumble of components connected by thin blue āRatlinesā. These lines represent the connections you need to make.
This is an art form.
Place Connectors First: USB ports, screw terminals, and headers should be on the edge of the board.
Core Components Center: The NodeMCU goes in the middle.
Keep Paths Short: Rotate the OLED and Relay so their pins face the NodeMCU pins they connect to.
Bad: Relay pin facing North, ESP pin facing South (Trace has to loop around).
Select the āBoardOutLineā layer (Pink). Draw a rectangle around your components.
Constraint: Make it small to save money, but leave breathing room for screws.
Mounting Holes: Place four 3mm holes in the corners for M3 screws.
Now we replace the āRatlinesā with real Copper Traces. Select āRouteā -> āTrackā.
How wide should a line be? Itās physics. Current flows through copper copper has resistance resistance creates heat ().
Signal Traces (Data): (10 mil). These carry almost zero current (micro-amps). Thin is fine.
Power Traces (5V, GND, Relay Coil): 0.5mm - 1.0mm.
The Calculation:
1 Amp current.
1oz Copper (Standard thickness: 35 micrometers).
Allowed Temp Rise: 10Ā°C.
Result: You need at least 0.3mm (12 mil). We use 0.5mm for safety.
Why? If you pull 1 Amp through a hair-thin trace (6 mil), it will heat up, delaminate from the fiberglass, and burn (Fusing Current).
Pro Tip: Use a Ground Plane (Copper Pour). Instead of routing Ground wires, we pour copper over the entire unused space of the board and connect it to GND.
Select āCopper Areaā.
Assign Net: GND.
Draw a box around the whole board.
Benefit 1: Low Impedance Return Path. Current wants to return to the source via the path of least impedance. A giant sheet of copper is near-zero impedance.
Benefit 2: EMI Shielding. The ground plane acts as a faraday cage, absorbing stray RF noise.
Benefit 3: Cooling. The entire board acts as a heatsink.
We have a 2-Layer board (Top and Bottom). Sometimes tracks cross. You cannot cross two tracks on the same layer. The Solution: A Via. It is a drilled hole (typically 0.4mm diameter) plated with copper that connects the Top Layer to the Bottom Layer.
For DC, current takes the path of least resistance. For High Frequency (Wi-Fi 2.4GHz), current takes the path of Least Inductance. This means the return current on the Ground Plane will hug directly underneath the signal trace on the top layer.
Critical Rule: Do not cut your Ground Plane! If you run a long track on the bottom layer that slices the Ground Plane in half, the return current has to take a huge detour loop. This creates a Loop Antenna, radiating noise and ruining your Wi-Fi signal. Keep your Ground Plane solid.
You will see 100nF (0.1uF) capacitors next to every microchip power pin.
The Solution: A small capacitor placed right next to the pin provides instant power.
Placement Rule: You MUST route power through the capacitor pad before it hits the chip pin. Distance matters.
If you design a standalone ESP8266, you have a 26MHz Crystal.
Length Matching: The two tracks (XTAL_IN, XTAL_OUT) must be exactly the same length.
Guard Ring: Surround these tracks with Ground Vias to shield them from noise.
Why? If the clock signal is jittery, your Wi-Fi will fail to connect.
Before you manufacture, you must run the DRC. This checks your board against the factoryās capabilities (JLCPCB rules).
Min Trace Width: 6 mil (0.15mm).
Min Clearance: 6 mil.
Min Drill Size: 0.3mm.
If you put two tracks 0.01mm apart, the factory cannot etch that. They will short circuit. The DRC will flag this with a big red āXā. Fix every single error.
The factory doesnāt want your EasyEDA project file. They want Gerber Files.
A Gerber file is like a PDF for machines. It tells the laser diagram plotter exactly where to draw.When you hold a PCB, you are looking at a sandwich:
Silkscreen (White): The text. SilkTop.gbr. Purely for humans.
Solder Mask (Green): The protective lacquer. MaskTop.gbr. It prevents solder bridges and protects copper from oxidation.
Copper (Shiny): The actual conductive path. TopLayer.gbr and BottomLayer.gbr.
Substrate (FR4): The yellow fiberglass body. Non-conductive.
You will be asked to choose a finish.
Pros: Perfectly flat, oxidation resistant, looks premium.
Cons: Expensive.
Recommendation: For this project (Relays, THT parts), HASL is perfect.
Export Steps:
File -> Generate PCB Fabrication File (Gerber).
Download the ZIP.
Critical Step: Open a Gerber Viewer (like Reference 3D or the JLCPCB viewer) to visually inspect one last time.
Check: Do you have Solder Mask openings over your pads? (If not, you canāt solder them).
| Component | Package | Quantity | Purpose |
|---|---|---|---|
| NodeMCU | DIP-30 | 1 | The brain. |
| 5V Relay | SRD-05VDC | 1 | High-voltage switch. |
| 2N2222 Transistor | TO-92 | 1 | Relay driver. |
| 1N4007 Diode | DO-41 | 1 | Flyback protection. |
| 1k Resistor | 0805 | 2 | Current limiting. |
| Screw Terminal | 5.08mm | 2 | Power & load. |
When browsing LCSC, you see resistor sizes: 0402, 0603, 0805, 1206.
Capacitor Voltage Rating: Always choose a voltage rating 2x your operating voltage.
One of the coolest features of modern EDA tools is the 3D View. Click ā3D Viewā. You will see a photorealistic render of your board. Look closely at:
Component Height: Will the Relay block the USB port?
Silkscreen: Is the text ā5Vā readable, or is it under a resistor?
Physical Clash: Are the screw terminals facing outwards? (Common newbie mistake: Putting terminals facing inwards so you canāt put wires in).
Before you order, perform this physical audit:
USB Port Clearance: Plug a real USB cable into your NodeMCU. Measure the plastic head width. Does it hit the Relay?
Screw Head Diameter: An M3 screw has a head diameter of ~5.5mm. Do you have copper traces too close to the mounting hole? The screw head will scrape the solder mask and short the trace to the case.
Tall Components: The Relay is 20mm tall. If you put this board in a 15mm slim case, the lid wonāt close.
You go to a manufacturer (JLCPCB, PCBWay, OSHPark).
Upload the Gerber ZIP.
Select Settings:
Layers: 2.
Dimensions: (Auto-detected).
PCB Thickness: 1.6mm (Standard).
PCB Color: Green (Fastest), Black (Coolest, but harder to trace debug), Blue, Red.
Surface Finish: HASL (Solder) or ENIG (Gold - flatter, expensive). For DIY, HASL is fine.
Price: Usually $2 for 5 boards + Shipping.
Wait 1 Week. When the package arrives, you have graduated. You hold in your hand a fiberglass/copper sandwich that you designed.
Even pros make mistakes. Here are the āBig Threeā to avoid:
When two tracks meet at an acute angle (less than 90Ā°), the etching acid gets trapped in the corner during manufacturing. It eats away the copper over time, causing an open circuit weeks later.
If one pad of a resistor has a massive copper trace (heatsink) and the other has a tiny trace, the massive one heats up slower during reflow. The solder melts on the small pad first, pulling the component upright like a tombstone.
You place a connector on the bottom layer, but forget to mirror the pinout. Now VCC connects to GND.
Q: Why not use KiCad? A: KiCad is excellent and Open Source. However, for a beginner, the learning curve is steep. EasyEDA handles the Library and LCSC integration seamlessly, removing friction. Once you master PCB concepts, switching to KiCad is easy.
Q: Can I mill this on a CNC at home? A: Yes, but it is messy (fiberglass dust is dangerous) and lacks Plated Through Holes (Vias). For $2, the factory quality is unbeatable.
Q: What is the āSilkscreenā limit? A: Most cheap fabs canāt print text smaller than 0.8mm high. If you go smaller, it becomes a blurry blob.
Q: My board arrived and it doesnāt work. Why? A: Did you run the DRC? Did you verify the Netlist? 99% of errors are in the Schematic. If the generic netlist says Pin 1 connects to Pin 2, the PCB software will force you to do it, even if itās wrong electrically.
We have moved from āDoes it work?ā to āIs it manufacturable?ā. You now possess the skill to create custom hardware.
Next Steps:
SMD Soldering: We focused on Through-Hole (THT) mostly. Next, try Surface Mount Devices (SMD) like 0805 resistors. They are tiny but cheaper.
Custom Microcontrollers: Instead of a NodeMCU module, design the bare ESP8266-12F chip directly onto your board (requires 3.3V LDO, USB-UART bridge logic).
High Power: Designing traces for 220V AC (Creepage and Clearance rules becomes critical).
Your Assignment: Design a āShieldā for the NodeMCU that holds the relay and OLED, eliminating all wires. Order it. Build it.
Copyright Ā© 2026 TechnoChips. Open Source Hardware (OSHW).
Stop relying on messy breadboards. Learn the professional developer's workflow for PCB design, from schematic capture to Gerber generation and manufacturing.
Read More ā