ATmega328P Breakout Board: Through-Hole PCB from Scratch

Modified: Mar. 5, 2026

Published: Mar. 5, 2026

Become Contributor Expert Support

In this first lesson, you will design a complete ATmega328P breakout board in KiCad 9 and produce files ready for home etching. The board is small (50x40mm), uses only through-hole components, and runs the same chip as an Arduino Uno. By the end you will have a working PCB with a blinking LED, built from scratch without any Arduino board or bootloader. #KiCad #ATmega328P #PCBDesign

What We Are Building

Board specifications:

Bill of Materials

Installing KiCad 9

# Ubuntu/Debian
sudo add-apt-repository ppa:kicad/kicad-9.0-releases
sudo apt update
sudo apt install kicad

# Fedora
sudo dnf install kicad

# Arch
sudo pacman -S kicad kicad-library

Verify the installation by opening KiCad. You should see the project manager with options for Schematic Editor, PCB Editor, and other tools.

Project Setup

1. Open KiCad 9 and click File > New Project.

2. Name the project atmega328p-breakout and choose a location. KiCad creates a .kicad_pro project file, a .kicad_sch schematic file, and a .kicad_pcb board file.

3. Open the Schematic Editor by double-clicking the .kicad_sch file in the project tree.

Schematic Capture

The schematic defines what components are on the board and how they connect. We will build it section by section.

Power Supply

The power section takes 7-12V from the barrel jack, regulates it to 5V, and provides decoupled power rails.

1. Place the barrel jack. Press A (Add Symbol), search for Barrel_Jack_Switch, and place it on the left side of the sheet. The barrel jack has three pins: Tip (positive), Sleeve (ground), and Switch (we leave this unconnected).

2. Place the voltage regulator. Add AMS1117-5.0 (search for AMS1117 in the symbol library). If your library has the generic LM1117-5.0, that works too. Place it to the right of the barrel jack.

3. Place capacitors. Add two C_Polarized symbols for C5 (10 µF, regulator input) and C6 (10 µF, regulator output). Place C5 between the barrel jack and regulator input, C6 between the regulator output and the MCU power pins.

4. Add power symbols. Press P (Add Power Port) and place +5V and GND symbols. Connect +5V to the regulator output and GND to the ground rail.

5. Wire everything. Press W to draw wires. Connect:

   • Barrel jack Tip to C5 positive to regulator VIN
   • Regulator VOUT to C6 positive to +5V
   • Barrel jack Sleeve, C5 negative, regulator GND, C6 negative all to GND

MCU and Crystal

1. Place the ATmega328P. Add ATmega328P-PU. This is the DIP-28 package variant. Place it in the center of the sheet.

2. Connect power pins. Wire VCC (pin 7) and AVCC (pin 20) to +5V. Wire GND (pins 8 and 22) to GND.

3. Place decoupling capacitors. Add two C symbols (100 nF each). Place C3 near VCC and C4 near AVCC. Connect each between the power pin and GND. These are critical for stable MCU operation.

4. Place the crystal. Add Crystal and place it near XTAL1 (pin 9) and XTAL2 (pin 10). Connect the crystal pins to XTAL1 and XTAL2.

5. Place crystal load capacitors. Add two C symbols (22 pF each, C1 and C2). Connect one from XTAL1 to GND and one from XTAL2 to GND.

6. AREF pin. Add a 100 nF capacitor from AREF (pin 21) to GND. This filters the analog reference voltage.

Reset Circuit

1. Place the pull-up resistor. Add R (10 kΩ, R1). Connect one end to the RESET pin (pin 1) and the other to +5V. This keeps the MCU running; pulling RESET low resets it.

2. Place the reset button. Add SW_Push. Connect one side to RESET and the other to GND. Pressing the button pulls RESET low.

ISP Programming Header

The 6-pin ISP header lets you program the ATmega328P using a USBasp programmer or an Arduino acting as ISP.

1. Place a 2x3 connector. Add Conn_AVR_ISP (or Conn_02x03_Odd_Even). This is the standard AVR ISP pinout.

2. Wire the ISP signals:

   • Pin 1 (MISO) to PB4 (pin 18)
   • Pin 2 (VCC) to +5V
   • Pin 3 (SCK) to PB5 (pin 19)
   • Pin 4 (MOSI) to PB3 (pin 17)
   • Pin 5 (RESET) to RESET (pin 1)
   • Pin 6 (GND) to GND

LEDs

1. Power LED. Add LED (D1) and R (R2, 330 Ω). Connect +5V to R2, R2 to D1 anode, D1 cathode to GND.

2. User LED. Add LED (D2) and R (R3, 330 Ω). Connect PB5 (pin 19) to R3, R3 to D2 anode, D2 cathode to GND. PB5 is the classic Arduino D13 pin.

I/O Pin Headers

1. Place two 1x14 connectors. Add Conn_01x14_Pin for J3 and J4. Place them on the left and right edges of the schematic.

2. Wire J3 to the left-side MCU pins: PD0-PD7 (pins 2-6, 11-13) and PB0-PB5 (pins 14-19).

3. Wire J4 to the analog/remaining pins: PC0-PC5 (pins 23-28), plus +5V, GND, AREF, and RESET for convenience.

Assign Component Values

Before leaving the schematic editor, assign values to every component:

1. Double-click each component to open its properties.

2. Set the Value field:

   • C1, C2: 22pF
   • C3, C4: 100nF
   • C5, C6: 10uF
   • R1: 10k
   • R2, R3: 330
   • Y1: 16MHz

3. Run Inspect > Electrical Rules Check (ERC). Fix any errors (unconnected pins, missing power flags). The ERC should pass with zero errors before you proceed.

Assign Footprints

Every schematic symbol needs a physical footprint for the PCB.

Open Tools > Assign Footprints (or click the footprint assignment icon in the toolbar) and assign each symbol its physical footprint:

Click Apply, Save Schematic & Continue, then close the footprint assignment dialog.

PCB Layout

Now we translate the schematic into a physical board.

Import Netlist

1. In the Schematic Editor, run Tools > Update PCB from Schematic (or press F8). This opens the PCB Editor and imports all components with their connections (the netlist).

2. All components appear stacked in one corner. Click to place them roughly in the center of the board.

Define Board Outline

1. Select the Edge.Cuts layer in the Layers panel.

2. Use Place > Rectangle to draw a 50 x 40 mm rectangle. You can type exact coordinates: start at (0, 0), end at (50, 40), or use the coordinate entry fields.

3. Round the corners if you want: select the rectangle, right-click, and choose Set Corner Radius (1 mm works well).

Component Placement

Good placement is the most important step in PCB layout. Place components logically before routing any traces.

1. Barrel jack on the left edge, oriented so the plug inserts from outside the board.

2. Voltage regulator near the barrel jack, with its input and output capacitors (C5, C6) close by.

3. ATmega328P in the center. Orient it so pin 1 is at the top-left. Use a DIP socket in your actual build for easy chip replacement.

4. Crystal and load caps (Y1, C1, C2) as close to XTAL1/XTAL2 (pins 9, 10) as possible. Keep the traces short to minimize noise pickup.

5. Decoupling caps (C3, C4) immediately next to the VCC and AVCC pins. The trace from the cap to the power pin should be as short as possible.

6. ISP header (J2) near the MCU, accessible from the board edge for easy programmer connection.

7. Reset button near the ISP header or board edge.

8. LEDs and resistors along one edge where they are visible.

9. Pin headers (J3, J4) on the left and right edges, making the board breadboard-friendly (2.54mm pitch, 15.24mm apart for standard breadboard rails).

Design Rules

Before routing, set up design rules appropriate for home etching:

1. Open Board Setup > Design Rules > Net Classes.

2. Set the Default net class:

   • Track width: 0.5 mm (generous for etching, about 20 mil)
   • Clearance: 0.3 mm (12 mil)
   • Via size: 0.8 mm (drill 0.4 mm), though we will avoid vias on a single-sided board

3. Add a Power net class for +5V and GND:

   • Track width: 0.8 mm (wider for current-carrying traces)
   • Clearance: 0.3 mm

4. Click OK to save the rules.

Routing

1. Route power first. Press X to start routing. Connect all +5V and GND traces first, using the wider Power net class. Route GND on the bottom copper layer if needed, but try to keep everything on one side for etching.

2. Route the crystal. Keep XTAL1 and XTAL2 traces short and parallel, away from other signals. This is the most noise-sensitive part of the circuit.

3. Route ISP signals. MISO, MOSI, SCK, and RESET from the MCU to the ISP header. Keep them reasonably short.

4. Route remaining signals. Connect the LEDs, reset button, and pin headers. The interactive router (press X and click pads) will push existing traces out of the way.

5. Add a ground pour. Select the F.Cu layer, then Place > Zone. Click the four corners of the board outline, select GND as the net, and press B to fill the zone. This connects all ground pads with a copper fill, improving noise immunity and making etching easier (less copper to remove).

6. Run DRC. Open Inspect > Design Rules Check and click Run DRC. Fix any errors. Common issues:

   • Unconnected pads (missed a trace)
   • Clearance violations (traces too close together)
   • Unrouted nets (the ratsnest lines still showing)

   The DRC should pass with zero errors and zero unconnected items.

3D Preview

Before manufacturing, check the 3D view:

1. Press Alt+3 or go to View > 3D Viewer.

2. Visually inspect:

   • Are all components on the correct side?
   • Does the barrel jack orient correctly?
   • Do the pin headers align for breadboard use?
   • Is there enough clearance between tall components?

3. Rotate the view to check from all angles. This catches placement mistakes that are invisible in the 2D view.

Manufacturing: Home Etching

For this first board, we will use the toner transfer method for home etching. This is the most accessible way to make a PCB without ordering from a fab house.

Generate Manufacturing Files

1. Export the copper layer as PDF. Go to File > Plot. Select only F.Cu (front copper). Set output format to PDF. Check Mirrored (because we will transfer the toner to the copper). Click Plot.

2. Export the drill file. In the Plot dialog, click Generate Drill Files. Select Excellon format. Click Generate Drill File. This tells you where to drill holes.

3. Export silkscreen (optional). Plot F.SilkS as a separate PDF for reference. You can transfer it to the board after etching if you want component labels.

Toner Transfer Process

1. Print the copper layer PDF on glossy magazine paper (or dedicated toner transfer paper) using a laser printer. The print must be mirrored so it reads correctly when transferred.

2. Prepare the copper board. Cut a single-sided copper-clad board to 50 x 40 mm. Clean the copper surface with fine sandpaper (400-600 grit) and isopropyl alcohol. The surface must be spotless for the toner to stick.

3. Transfer the toner. Place the printed side of the paper face-down on the clean copper. Iron over it with a clothes iron set to maximum heat (no steam) for about 5 minutes, applying firm, even pressure. Let it cool, then soak in warm water and gently peel the paper away. The toner stays on the copper.

4. Etch the board. Submerge the board in ferric chloride solution (available at electronics stores). Agitate gently. The exposed copper dissolves in 10-30 minutes depending on temperature and concentration. The areas protected by toner remain as traces.

5. Clean the board. Remove the board when all exposed copper is gone. Rinse with water. Remove the remaining toner with acetone or fine sandpaper.

6. Drill the holes. Use a 0.8 mm drill bit for component leads and a 1.0 mm bit for pin headers and the barrel jack. A drill press or hand drill with a PCB drill bit works. Use the drill file as a reference for hole positions.

7. Inspect the board. Check for:

   • Broken traces (fix with a thin wire and solder)
   • Short circuits between traces (scrape away with a craft knife)
   • Clean, properly-sized holes

Soldering and Assembly

1. Install the DIP socket first. Solder the 28-pin DIP socket for U1. This lets you remove the ATmega328P without desoldering. Align the notch with pin 1.

2. Solder low-profile components next. Resistors (R1, R2, R3), ceramic capacitors (C1-C4), and the crystal (Y1).

3. Then taller components. Electrolytic capacitors (C5, C6, watch polarity), LEDs (D1, D2, longer leg is anode/positive), the reset button (SW1).

4. Connectors last. Barrel jack (J1), ISP header (J2), pin headers (J3, J4). These are the tallest components.

5. Voltage regulator. Solder U2 (AMS1117-5.0). If using the SOT-223 surface-mount version, solder it on the bottom of the board. If using TO-220 through-hole, it goes on top with a small heat sink if needed.

6. Insert the ATmega328P into the DIP socket. Match pin 1 (marked with a dot on the chip) with the socket notch.

First Power-On

1. Visual inspection. Before applying power, check every solder joint under magnification. Look for solder bridges (shorts between adjacent pins) and cold joints (dull, lumpy solder).

2. Continuity check. Use a multimeter in continuity mode. Verify:

   • No short between +5V and GND
   • +5V reaches VCC (pin 7) and AVCC (pin 20)
   • GND reaches pins 8 and 22

3. Apply power. Connect a 9V battery or 7-12V power supply to the barrel jack. The power LED (D1) should light up.

4. Measure voltages. With the multimeter, verify:

   • 5.0V (±0.1V) between +5V and GND
   • 5.0V at ATmega328P VCC (pin 7)
   • If the voltage is wrong, power off immediately and check the regulator connections.

Firmware: Blink LED

We will program the ATmega328P directly over ISP, without the Arduino IDE or bootloader. This proves the board works at the hardware level.

Toolchain Setup

sudo apt install avr-libc avrdude gcc-avr

brew install avr-gcc avrdude

Blink Code

Save this as blink.c:

/*
 * blink.c - Toggle LED on PB5 (pin 19) every 500ms
 * ATmega328P @ 16 MHz, no Arduino, no bootloader
 */

#define F_CPU 16000000UL

#include <avr/io.h>
#include <util/delay.h>

int main(void) {
    DDRB |= (1 << PB5);   /* Set PB5 as output */

    while (1) {
        PORTB ^= (1 << PB5);  /* Toggle PB5 */
        _delay_ms(500);
    }
}

Compile and Flash

Connect a USBasp programmer (or Arduino-as-ISP) to the 6-pin ISP header. The ribbon cable pin 1 should match the header pin 1.

# Compile
avr-gcc -mmcu=atmega328p -DF_CPU=16000000UL -Os -o blink.elf blink.c
avr-objcopy -O ihex blink.elf blink.hex

# Set fuses for 16 MHz external crystal
avrdude -c usbasp -p m328p -U lfuse:w:0xFF:m -U hfuse:w:0xDE:m -U efuse:w:0xFD:m

# Flash the program
avrdude -c usbasp -p m328p -U flash:w:blink.hex:i

If you are using an Arduino Uno as an ISP programmer, replace -c usbasp with -c arduino -P /dev/ttyACM0 -b 19200 (adjust the port for your system).

The red user LED (D2) should now blink at 1 Hz (500ms on, 500ms off). If it does, your board is fully functional: power supply, crystal, MCU, and I/O all work.

What You Have Learned