Design a 5V/1A DC-DC Buck Converter PCB

Simulate, design, fabricate, and test a 12V-to-5V buck converter PCB.

Introduction

30 Second Summary

Every electronic device you own has a power supply converting voltage from one level to another. From phone chargers to laptops, buck converters are the most common circuit topology making this happen.

In this project, you will design, simulate, and build a 12V-to-5V DC-DC buck converter PCB from scratch. You'll take it through the full electronics design workflow: requirements, simulation, schematic capture, layout, fabrication, and bench testing.

What You'll Build

A complete 12V-to-5V, 1A synchronous buck converter based on the Texas Instruments TPS561208DDCR, designed in KiCad and validated with LTspice simulation before fabrication.

By the end of this project, you'll have:

  • A fully simulated buck converter circuit in LTspice with verified output voltage, ripple, and transient response waveforms.
  • A manufactured, assembled, and tested 5V/1A buck converter PCB designed in KiCad with proper power electronics layout techniques.
  • A documented design portfolio piece with schematic, simulation results, PCB layout screenshots, and test measurements ready for your CV.
  • Secret Mission: Add an LED power-good indicator and USB-A output connector to turn your converter into a functional USB charger.

Are there any prerequisites?

You should be comfortable with basic circuit theory: Ohm's law, voltage dividers, and how inductors and capacitors behave. A basic understanding of what DC-DC conversion means is helpful, but you do not need prior experience with PCB design or SPICE simulation.

Define Requirements and Select Components

Before touching a schematic or PCB layout, professional engineers lock down their design requirements and select components. This prevents costly mid-design changes when a part turns out to be wrong for the job.

In this step, you will define the electrical specification for your buck converter, select the IC and passive components based on datasheet recommendations, then compile a Bill of Materials ready for ordering.

In this step, get ready to:
  • Document the design requirements for a 12V-to-5V, 1A buck converter.
  • Calculate the feedback resistor divider and select the inductor and capacitors.
  • Create a complete Bill of Materials with distributor part numbers.
Document the design requirements and select the converter IC

Every power supply design starts with a requirements specification. This tells you exactly what the circuit must deliver and constrains every component choice you make afterwards.

  • Open a text editor (or a blank document in any note-taking app) and record the following design requirements:
# Buck Converter Design Requirements
# -----------------------------------
# Input voltage:       7V - 12V (nominal 12V)
# Output voltage:      5.0V
# Output current:      1A (max)
# Output ripple:       < 50 mV peak-to-peak
# Switching frequency: 580 kHz
# Topology:            Synchronous buck (step-down)

Why these specific values?

A 12V input represents common bench supplies and automotive accessory rails. A 5V/1A output is the same rail that powers USB devices, microcontrollers, and sensors.

The 50 mV ripple target ensures clean power for sensitive digital logic. The 580 kHz switching frequency keeps the inductor and capacitors small without sacrificing too much efficiency.

  • Based on these requirements, select the TPS561208DDCR from Texas Instruments as the converter IC.

Why the TPS561208?

The TPS561208DDCR is a 4.5V to 17V input, 1A synchronous step-down converter in a 6-pin SOT-23 package. It uses D-CAP2 control mode, which means no external compensation components are needed.

The SOT-23-6 package is large enough to hand-solder. It has extensive documentation from TI including an evaluation module with a known-good BOM. These qualities make it ideal for a first SMPS project.

Calculate the feedback divider and select passive components

The TPS561208 uses a resistor divider on its FB pin to set the output voltage. You need to calculate exact resistor values, then choose an inductor and capacitors that meet the ripple and current requirements.

  • Calculate the feedback resistor divider using the datasheet formula:
# Feedback Divider Calculation
# Formula: VOUT = VFB x (1 + R1/R2)
# VFB (typical) = 0.768V (from datasheet)
#
# For VOUT = 5.0V:
#   5.0 = 0.768 x (1 + R1/R2)
#   1 + R1/R2 = 5.0 / 0.768 = 6.51
#   R1/R2 = 5.51
#
# Choose R2 = 10 kΩ (standard value)
#   R1 = 5.51 x 10 kΩ = 55.1 kΩ
#   Nearest standard 1% E96 value: 54.9 kΩ
#
# Verify: VOUT = 0.768 x (1 + 54.9/10) = 0.768 x 6.49 = 4.986V ≈ 5.0V (within 2%)

What is a feedback voltage divider?

The TPS561208 regulates its output by monitoring a scaled-down version of VOUT through two resistors (R1 on top, R2 on the bottom). It adjusts switching until the FB pin voltage equals its internal reference of 0.768V.

Choosing standard 1% tolerance resistors ensures the output stays within the 2% accuracy specification of the IC.

  • Record the following component selections based on the TPS561208 evaluation module design:
# Passive Component Selection
# ----------------------------
# INDUCTOR:
#   L1 = 2.2 µH, shielded SMD drum core
#   Saturation current >= 1.5A (choose part rated for 9A+ for margin)
#   Part: Wurth Elektronik 744311220 (WE-HCI series, Isat = 13A)
#
# INPUT CAPACITORS:
#   C_IN1, C_IN2 = 10 µF, 25V rated, X5R dielectric, 1206 package
#   Part: Murata GRM31CR61E106KA12L
#
# OUTPUT CAPACITORS:
#   C_OUT1, C_OUT2 = 22 µF, 10V rated, X7R dielectric, 1206 package
#   Part: Murata GRM31CR71A226KE15L
#
# BOOTSTRAP CAPACITOR:
#   C_BST = 0.1 µF, 25V rated, X5R, 0603 package
#   Part: Murata GRM188R61E104KA01D
#
# INPUT BYPASS/DECOUPLING:
#   C_BYPASS = 0.1 µF, 25V, X5R, 0603
#   Part: Murata GRM188R61E104KA01D

Why these specific parts?

Every passive component here comes from the TPS561208EVM-896 evaluation module BOM published by Texas Instruments. Using proven reference-design values removes guesswork on your first converter project.

The inductor's 13A saturation rating gives massive margin over the 1A output. This prevents inductance droop under load transients that would cause output voltage sag.

Create the Bill of Materials with distributor part numbers

A BOM (Bill of Materials) is the ordering list that maps every schematic component to a real purchasable part. You will use this to order components from DigiKey, Mouser, or LCSC.

  • Inside your buck-converter-5v1a project folder, create a file called BOM.csv and paste the following content:
Reference,Value,Package,Description,DigiKey,Mouser,LCSC
IC1,TPS561208DDCR,SOT-23-6,Synchronous Buck Converter 4.5-17V 1A,296-47886-1-ND,595-TPS561208DDCR,C138335
R1,54.9 kΩ 1%,0603,Feedback top resistor,311-54.9KHRCT-ND,71-CRCW060354K9FKEAC,C23196
R2,10 kΩ 1%,0603,Feedback bottom resistor,311-10.0KHRCT-ND,71-CRCW060310K0FKEAC,C25804
C_IN1,10 µF 25V X5R,1206,Input capacitor,490-GRM31CR61E106KA12L,81-GRM31CR61E106KA2L,C13585
C_IN2,10 µF 25V X5R,1206,Input capacitor,490-GRM31CR61E106KA12L,81-GRM31CR61E106KA2L,C13585
C_OUT1,22 µF 10V X7R,1206,Output capacitor,490-GRM31CR71A226KE15L,81-GRM31CR71A226KE5L,C59461
C_OUT2,22 µF 10V X7R,1206,Output capacitor,490-GRM31CR71A226KE15L,81-GRM31CR71A226KE5L,C59461
C_BST,0.1 µF 25V X5R,0603,Bootstrap capacitor,490-GRM188R61E104KA01D,81-GRM188R61E104KA1D,C14663
C_BYPASS,0.1 µF 25V X5R,0603,Input decoupling capacitor,490-GRM188R61E104KA01D,81-GRM188R61E104KA1D,C14663
L1,2.2 µH WE-HCI,7040,Shielded power inductor 9A,732-1151-1-ND,710-744311220,C2651184
J1,Terminal Block 2-pin,5.08mm pitch,Input connector,ED10561-ND,651-1729128,C8465
J2,Terminal Block 2-pin,5.08mm pitch,Output connector,ED10561-ND,651-1729128,C8465

What do the distributor codes mean?

Each row maps one schematic component to a real part you can buy. DigiKey codes like 296-47886-1-ND are their internal order numbers. Mouser uses codes like 710-744311220. LCSC codes like C138335 are used with JLCPCB assembly.

Having all three distributors listed means you can order from whichever has stock and the best shipping to your region.

  • Save BOM.csv in your project folder.
  • Open BOM.csv in your text editor and confirm it has 12 component rows (IC1, R1, R2, C_IN1, C_IN2, C_OUT1, C_OUT2, C_BST, C_BYPASS, L1, J1, J2).

Can't find a part on your chosen distributor?

Component availability changes frequently. If a specific Murata capacitor is out of stock, search for the same value, voltage rating, dielectric, and package size from another manufacturer (Samsung, Yageo, TDK). The critical parameters are capacitance, voltage rating, dielectric type (X5R/X7R), and package.

For the TPS561208DDCR specifically, do not substitute a different IC without recalculating the feedback network and checking pin compatibility.

help me find equivalent components for my buck converter BOM

✔️ Awesome, I've got everything!

Great. Double check you have saved BOM.csv in your buck-converter-5v1a project folder.

ⓧ I'd like to double check the full BOM

Here is the complete BOM for comparison:

Reference,Value,Package,Description,DigiKey,Mouser,LCSC
IC1,TPS561208DDCR,SOT-23-6,Synchronous Buck Converter 4.5-17V 1A,296-47886-1-ND,595-TPS561208DDCR,C138335
R1,54.9 kΩ 1%,0603,Feedback top resistor,311-54.9KHRCT-ND,71-CRCW060354K9FKEAC,C23196
R2,10 kΩ 1%,0603,Feedback bottom resistor,311-10.0KHRCT-ND,71-CRCW060310K0FKEAC,C25804
C_IN1,10 µF 25V X5R,1206,Input capacitor,490-GRM31CR61E106KA12L,81-GRM31CR61E106KA2L,C13585
C_IN2,10 µF 25V X5R,1206,Input capacitor,490-GRM31CR61E106KA12L,81-GRM31CR61E106KA2L,C13585
C_OUT1,22 µF 10V X7R,1206,Output capacitor,490-GRM31CR71A226KE15L,81-GRM31CR71A226KE5L,C59461
C_OUT2,22 µF 10V X7R,1206,Output capacitor,490-GRM31CR71A226KE15L,81-GRM31CR71A226KE5L,C59461
C_BST,0.1 µF 25V X5R,0603,Bootstrap capacitor,490-GRM188R61E104KA01D,81-GRM188R61E104KA1D,C14663
C_BYPASS,0.1 µF 25V X5R,0603,Input decoupling capacitor,490-GRM188R61E104KA01D,81-GRM188R61E104KA1D,C14663
L1,2.2 µH WE-HCI,7040,Shielded power inductor 9A,732-1151-1-ND,710-744311220,C2651184
J1,Terminal Block 2-pin,5.08mm pitch,Input connector,ED10561-ND,651-1729128,C8465
J2,Terminal Block 2-pin,5.08mm pitch,Output connector,ED10561-ND,651-1729128,C8465

Your requirements are locked in and every component has a part number ready to order. Next up, you will bring this circuit to life in LTspice and simulate its switching behaviour before committing to a PCB.

Simulate the Buck Converter in LTspice

Your components are selected and your BOM is complete. Now it's time to verify the design works before committing to a physical PCB.

Simulation lets you catch errors early and build confidence that the LC filter produces the right output voltage and ripple. You'll build an ideal buck converter model in LTspice to confirm your power stage meets every design target.

In this step, get ready to:
  • Build an ideal buck converter schematic in LTspice with a PWM source, switch, diode, and LC filter.
  • Run a transient simulation and verify steady-state output voltage, ripple, and inductor current.
  • Perform a load transient test and document all results with screenshots.
Build the ideal buck converter schematic in LTspice

The TPS561208 does not have a downloadable SPICE model in LTspice's built-in library. Instead, you'll build an ideal buck converter model using a voltage-controlled switch, freewheeling diode, and passive LC filter.

This approach validates the power stage fundamentals (output voltage, ripple, inductor current) without getting blocked on model availability.

  • Press Cmd+Space (macOS) or the Windows key (Windows) to open your search bar.
  • Type LTspice and press Enter to open it.
  • Create a new schematic by clicking File in the menu bar, then New Schematic.

You'll place seven components to form the complete buck converter power stage. Here's the circuit topology:

  • V_IN (12V DC supply) provides the input power.
  • V_PWM (PULSE source) generates the switching signal at 580 kHz.
  • S1 (voltage-controlled switch) acts as the ideal MOSFET, connecting VIN to the SW node.
  • D1 (Schottky diode) freewheels inductor current when the switch is off.
  • L1 (2.2 µH inductor) stores energy and smooths current.
  • C1 and C2 (22 µF output capacitors) filter the output voltage ripple.
  • R_LOAD (5 Ω) represents your 1A load at 5V.
  • Place the 12V DC voltage source by pressing P to open the component browser, searching for voltage, and placing it on the schematic.
  • Right-click the voltage source and set its value to 12.
  • Place a second voltage source for the PWM signal.
  • Right-click the PWM source, click Advanced, select PULSE, and enter the following parameters:
Vinitial: 0
Von: 12
Tdelay: 0
Trise: 1n
Tfall: 1n
Ton: 724n
Tperiod: 1.724u

What do these PULSE parameters mean?

  • Vinitial and Von set the low and high voltage levels (0V to 12V swing).
  • Trise and Tfall of 1 ns model near-ideal fast switching edges.
  • Ton of 724 ns is approximately 42% of the period. This gives duty cycle D = 5V/12V = 0.42.
  • Tperiod of 1.724 µs corresponds to 1/580 kHz, matching the TPS561208 switching frequency.
  • Place the voltage-controlled switch by pressing P and searching for sw.
  • Connect the switch's positive terminal to the V_IN positive node and its negative terminal to the SW net.
  • Connect the switch's control terminals: control positive to the V_PWM output, control negative to ground.

The switch needs a model directive to define its on-resistance and threshold voltage.

  • Add the switch model by right-clicking on empty space, selecting Edit Simulation Cmd, and entering this SPICE directive as a text label on the schematic:
.model IDEAL_SW SW(Ron=0.01 Roff=1Meg Vt=2.5)

What does this model do?

Ron=0.01 gives the switch a 10 mΩ on-resistance (nearly ideal). Roff=1Meg makes it effectively open when off. Vt=2.5 means the switch closes when the control voltage exceeds 2.5V.

  • Place the diode by pressing P and searching for diode.
  • Connect the diode's anode to ground and its cathode to the SW net. This allows freewheeling current to flow when the switch turns off.
  • Add a Schottky diode model directive on the schematic:
.model SCHOTTKY D(Is=1e-5 Rs=0.01 N=1.05 BV=40)
  • Place the inductor by pressing P and searching for ind. Set its value to 2.2u.
  • Connect L1 from the SW net to the output net (label it VOUT).
  • Place two capacitors (search cap), each set to 22u. Connect both from VOUT to ground.
  • Place a resistor (search res), set its value to 5. Connect it from VOUT to ground.
  • Add ground symbols by pressing G and connecting them to all ground nodes (V_IN negative, diode anode, capacitor negatives, load resistor bottom).
  • Wire all connections using W (wire tool). Add net labels VIN, SW, and VOUT by pressing L (label net).
  • Save the schematic as buck_converter_sim.asc by clicking File then Save As. Save it on your Desktop alongside your KiCad project.

Wires not connecting?

LTspice requires wires to snap exactly to component pins. Zoom in with the scroll wheel and make sure each wire endpoint lands directly on a pin dot.

If you see dashed lines instead of solid connections, delete the wire and try again with a closer starting point.

Help me debug my LTspice schematic connections.

Run a transient simulation and verify performance

With the schematic complete, you'll run a time-domain transient simulation. This tells LTspice to compute voltages and currents over 10 milliseconds of switching activity.

  • Add the transient simulation command by clicking Simulate in the menu bar, then Edit Simulation Cmd.
  • In the Transient tab, enter 10m in the Stop time field.
  • Click OK. The directive .tran 10m appears on your schematic.
.tran 10m

Why 10 milliseconds?

At 580 kHz, 10 ms covers about 5,800 switching cycles. This gives the converter time to reach steady state (the first 1-2 ms is startup transient) and provides clean waveforms for measurement.

  • Run the simulation by clicking the Run button (green triangle) in the toolbar, or press Cmd+R (macOS) or Ctrl+R (Windows).
  • Wait for the simulation to complete. A waveform viewer window opens automatically.

Now you'll probe the three critical waveforms to verify your design meets spec.

  • Click on the VOUT net label in your schematic. The output voltage waveform appears in the viewer.
  • Zoom into the steady-state region (after 2 ms) by clicking and dragging a rectangle on the time axis.
  • Verify the output voltage settles to approximately 5.0V (within ±2%, so between 4.9V and 5.1V).

How to measure output ripple

Zoom in further on the VOUT waveform at steady state until you can see the small triangular ripple riding on top of the DC level. The peak-to-peak amplitude of this ripple should be less than 50 mV.

You can read precise values by hovering your cursor over the waveform peaks and troughs. LTspice displays the voltage at the cursor position in the status bar.

  • Probe the inductor current by clicking on L1 in your schematic. The current waveform appears.
  • Verify the inductor current shows a triangular waveform (ramp up during switch on, ramp down during switch off). This confirms continuous conduction mode (CCM).
  • If the current touches zero and stays flat, the converter is in discontinuous mode. Check that your Ton and Tperiod PULSE values are correct.
  • Take screenshots of all three verified waveforms (VOUT steady state, output ripple zoomed in, inductor current).
  • Create a folder called simulation_screenshots on your Desktop and save the screenshots there.

Output voltage is wrong or oscillating wildly?

  • Check the duty cycle. With Ton=724n and Tperiod=1.724u, the output should be approximately 12V x 0.42 = 5V. A typo in either value gives the wrong voltage.
  • Check that the diode is oriented correctly: anode to ground, cathode to the SW net. A reversed diode prevents the freewheeling path and causes wild oscillation.
  • Make sure the switch model directive .model IDEAL_SW SW(Ron=0.01 Roff=1Meg Vt=2.5) is placed directly on the schematic as a SPICE directive, not inside a comment.

Help me debug my buck converter simulation output.

Perform a load transient simulation

A real power supply must handle sudden changes in load current without the output voltage dropping too far. You'll step the load from 0.5A to 1A and measure how the converter responds.

  • Delete the 5 Ω load resistor from your schematic (click it and press Delete).
  • Place a current source by pressing P and searching for current. Connect its positive terminal to VOUT and negative terminal to ground.
  • Right-click the current source, click Advanced, select PWL, and enter the following piecewise linear values:
PWL(0 0.5 5m 0.5 5.001m 1 10m 1)

What does this PWL function do?

The current source draws 0.5A from time 0 to 5 ms, then steps abruptly to 1A at 5.001 ms (a 1 µs transition). It holds 1A until the simulation ends at 10 ms.

This simulates a sudden doubling of load current. The tiny 1 µs step mimics a real-world load transient that your converter must handle.

  • Run the simulation again by pressing Cmd+R (macOS) or Ctrl+R (Windows).
  • Probe the VOUT node to see the load transient response.
  • Look at the moment the load steps (around 5 ms on the time axis). You should see a brief voltage dip (undershoot) followed by a recovery back to 5V.
  • Measure the undershoot depth using the cursor (hover over the lowest point of the dip). Note this value for your test report.
  • Measure the recovery time from the dip to when the voltage returns within 2% of 5V (between 4.9V and 5.1V).
  • Take a screenshot of the load transient response showing the undershoot and recovery.
  • Save it in your simulation_screenshots folder.
  • Save the LTspice schematic (Cmd+S or Ctrl+S) to preserve the load transient version.

Keep both simulation variants

You can use File > Save As to save the load transient version as a separate file (e.g. buck_converter_sim_transient.asc). Then revert to the 5 Ω resistor version for your primary simulation file.

Your simulation_screenshots folder should now contain four images: steady-state VOUT, output ripple measurement, inductor current waveform, and load transient response.

✔️ Awesome, I've got everything!

Great. Make sure you've saved buck_converter_sim.asc and all four screenshots are in your simulation_screenshots folder.

ⓧ I'd like to double check the full circuit

Here's the complete SPICE netlist your graphical schematic represents. Verify each component and connection matches:

* Buck Converter Ideal Model - 12V to 5V, 1A

* 12V input supply
V_IN VIN 0 12

* PWM gate drive at 580 kHz, ~42% duty cycle
V_PWM PWM 0 PULSE(0 12 0 1n 1n 724n 1.724u)

* Ideal MOSFET switch (voltage-controlled)
S1 VIN SW PWM 0 IDEAL_SW
.model IDEAL_SW SW(Ron=0.01 Roff=1Meg Vt=2.5)

* Freewheeling Schottky diode (anode=GND, cathode=SW)
D1 0 SW SCHOTTKY
.model SCHOTTKY D(Is=1e-5 Rs=0.01 N=1.05 BV=40)

* Output LC filter
L1 SW VOUT 2.2u
C1 VOUT 0 22u
C2 VOUT 0 22u

* Load resistor (5 ohm = 1A at 5V)
R_LOAD VOUT 0 5

* Transient simulation for 10 ms
.tran 10m

Simulation runs forever or crashes?

LTspice may struggle if rise/fall times are set to exactly 0. Make sure Trise and Tfall are 1n (1 nanosecond), not 0.

If the simulation is very slow, check that you don't have extra unconnected components floating on the schematic. Delete any unused parts.

Help me fix my LTspice simulation performance.

Your simulation confirms the buck converter power stage meets all design targets. Next, you'll capture the full schematic with the TPS561208 in KiCad and prepare it for PCB layout.

Capture the Schematic in KiCad

Your simulation confirmed the buck converter design works on paper. Now it's time to turn that validated circuit into a real schematic that KiCad can use to generate a physical PCB.

In this step, you'll draw every component and connection in the KiCad Schematic Editor, matching the TPS561208 datasheet's typical application circuit. You'll also run the Electrical Rules Check to catch wiring mistakes before they become expensive PCB errors.

In this step, get ready to:
  • Draw the complete buck converter schematic with all components wired per the datasheet.
  • Annotate components and run ERC to verify zero errors.
  • Assign PCB footprints to every component.
Draw the buck converter circuit in the Schematic Editor

The schematic is the single source of truth for how every component connects. KiCad uses it to generate the netlist that drives the PCB layout.

  • Switch back to the KiCad Project Manager window (it should still be open from Step 1).
  • Double-click the buck-converter-5v1a.kicad_sch file in the project tree to open the Schematic Editor.
  • Click File in the menu bar, then Page Settings.
  • Enter Buck Converter 5V 1A - TPS561208 in the Title field and click OK.

Now place the TPS561208 IC symbol. This is the heart of your converter.

  • Press A on your keyboard to open the Choose Symbols dialog.
  • Type TPS561208 in the search field.
  • Select the TPS561208 symbol (in the Regulator_Switching library) and click OK.
  • Click in the centre of your schematic sheet to place the IC. Press Esc to stop placing.

What are the TPS561208 pins?

The TPS561208 in its SOT-23-6 package exposes six pins: VIN (power input), GND (ground), EN (enable), SW (switch node output), BST (bootstrap for high-side gate driver), and FB (feedback for output voltage sensing).

Your schematic will connect external components to each of these pins exactly as described in the datasheet's typical application circuit.

Next, place the passive components around the IC. You'll add them one group at a time.

  • Press A again to open the symbol chooser.
  • Search for C in the Device library. Select the capacitor symbol.
  • Place six capacitors on the schematic: two for input decoupling (C1, C2 at 10 µF), one input bypass (C3 at 0.1 µF), one bootstrap (C4 at 0.1 µF), and two output (C5, C6 at 22 µF). Arrange them near their respective IC pins.
  • Press A, search for R in the Device library, and place two resistors for the feedback divider (R1 at 54.9 kΩ, R2 at 10 kΩ).
  • Press A, search for L in the Device library, and place one inductor (L1 at 2.2 µH).
  • Press A, search for Conn_01x02 in the Connector_Generic library. Place two 2-pin connectors for J1 (input) and J2 (output).

Rotate before placing

Press R while a symbol is attached to your cursor to rotate it 90 degrees. This helps you orient resistors vertically for the feedback divider and keep wires tidy.

Now wire everything together following the TPS561208 typical application circuit.

  • Press W to activate the wire tool.
  • Connect J1 pin 1 to the VIN pin of IC1. Route a wire from VIN to the positive side of C1, C2, and C3 (all in parallel to GND).
  • Connect the EN pin directly to VIN (always-on configuration).
  • Connect C4 (0.1 µF) between the BST and SW pins.
  • Connect L1 from the SW pin to the output node (VOUT).
  • Connect C5 and C6 (both 22 µF) from VOUT to GND.
  • Connect R1 (54.9 kΩ) from VOUT to the FB pin. Connect R2 (10 kΩ) from FB to GND.
  • Connect J2 pin 1 to VOUT. Connect J1 pin 2 and J2 pin 2 to GND.

Finally, add net labels and power flags to keep the schematic clean and pass ERC.

  • Press L to place net labels. Add labels named VIN, VOUT, and SW on the appropriate nets.
  • Press P to open the power symbol chooser. Search for PWR_FLAG and place one on the VIN net and one on the GND net.
  • Press P again, search for GND, and place ground power symbols on every GND connection point.

Why add PWR_FLAG symbols?

KiCad's ERC checks that every power net has a source. Your input connector provides power in reality, but KiCad doesn't know that from the schematic alone. The PWR_FLAG symbol tells ERC that these nets are intentionally driven.

  • Save your schematic with Cmd+S (macOS) or Ctrl+S (Windows).

You should see IC1 in the centre with capacitors clustered around the VIN and VOUT rails, the inductor bridging SW to VOUT, and the feedback divider running from VOUT down to GND through the FB pin.

Wires not connecting?

KiCad only creates electrical connections at wire endpoints that land exactly on pins. If you see small circles on pin ends, the wire hasn't reached the pin. Zoom in and drag the wire endpoint onto the pin tip until the circle disappears.

Help me fix my dangling wire connections in the KiCad schematic editor.

Annotate components and run the Electrical Rules Check

Annotation assigns unique reference designators (IC1, R1, C1, etc.) to every symbol. The ERC then verifies that all pins are properly connected and no electrical rules are violated.

  • Click the Annotate Schematic button in the top toolbar (it looks like a sheet with "R1, R2" on it).
  • In the Annotation dialog, leave the default scope set to Entire schematic.
  • Click Annotate. KiCad assigns reference designators starting from 1 for each component type.
  • Click Close.

Now verify your schematic has no electrical errors.

  • Click the ERC button in the top toolbar (the button with a checkmark and bug icon).
  • In the Electrical Rules Checker dialog, click Run ERC.
  • Review the results. Your target is zero errors and zero warnings.

What does ERC check?

The Electrical Rules Check scans for common schematic mistakes: unconnected pins, two power outputs shorted together, a power input that has no source, unannotated symbols, and typos in net labels.

It cannot guarantee your circuit works, but it catches wiring mistakes that would be costly to fix on a manufactured PCB.

  • If ERC reports errors, double-click each error in the list to jump to the violation location. Fix missing connections or add PWR_FLAG symbols where needed.
  • Re-run ERC until it reports zero errors and zero warnings.
  • Save the schematic again with Cmd+S (macOS) or Ctrl+S (Windows).

Your ERC results panel should show a green checkmark with no violations listed.

ERC showing power pin errors?

The most common ERC error on power converter schematics is a power pin not driven. This happens when your VIN or GND net is missing a PWR_FLAG symbol. Place one on the VIN net near J1 and one on the GND net, then re-run ERC.

Help me resolve ERC power pin errors with PWR_FLAG in my KiCad schematic.

Assign PCB footprints to all components

Each schematic symbol needs a corresponding physical footprint that defines its pad layout on the PCB. KiCad uses these footprints when you transfer the design to the board editor.

  • Click the Assign Footprints button in the top toolbar (it shows a chip with an arrow to a footprint).
  • The Footprint Assignment Tool opens with three panes: libraries on the left, your schematic symbols in the middle, and available footprints on the right.

Assign the following footprints by selecting each symbol in the middle pane and double-clicking the correct footprint in the right pane:

  • IC1 (TPS561208): Package_TO_SOT_SMD:SOT-23-6.
  • R1, R2 (resistors): Resistor_SMD:R_0603_1608Metric.
  • C3, C4 (0.1 µF capacitors): Capacitor_SMD:C_0603_1608Metric.
  • C1, C2 (10 µF input caps): Capacitor_SMD:C_1206_3216Metric.
  • C5, C6 (22 µF output caps): Capacitor_SMD:C_1206_3216Metric.
  • L1 (2.2 µH inductor): Select an appropriate shielded SMD inductor footprint from the Inductor_SMD library that matches the physical dimensions of your chosen inductor from the BOM.
  • J1, J2 (connectors): Select a 2-pin terminal block footprint from the Connector_PinHeader_2.54mm or TerminalBlock library.

Use the pin count filter

Enable the middle filter button in the Footprint Assignment Tool to filter footprints by pin count. This dramatically narrows the list and makes it easier to find the correct footprint for each component.

  • Once all footprints are assigned, click OK to close the Footprint Assignment Tool.
  • Save the schematic with Cmd+S (macOS) or Ctrl+S (Windows).

To verify your footprint assignments, double-click any symbol in the schematic and check the Footprint field in its properties. Every component should show a footprint path.

Why these specific footprints?

The TPS561208 comes in a SOT-23-6 package. The 0603 footprint is used for the small-value passives (resistors, 0.1 µF caps) because they're easy to solder by hand at this size.

The 1206 footprint is used for the bulk capacitors (10 µF, 22 µF) because higher-capacitance ceramics need a larger case size to meet their voltage ratings.

Can't find the TPS561208 symbol or footprint?

KiCad's built-in libraries include thousands of components, but specific parts like the TPS561208 may need to be downloaded from the manufacturer. Check the KiCad library browser first. If it's not there, download the KiCad symbol and footprint from the TI website or a component library site like SnapEDA, and add them to your project library.

Help me add a custom TPS561208 symbol and footprint to my KiCad project.

Your schematic is now fully captured, validated, and ready for PCB layout. In the next step, you'll transfer this design to the PCB Editor and lay out the board with proper power electronics routing techniques.

Design the PCB Layout

Your schematic is complete and verified. Now it is time to turn that circuit into a physical board that can be manufactured.

In this step, you will transfer the schematic into the KiCad PCB Editor, place components to minimise the high-current switching loop, route power traces at appropriate widths, and generate the manufacturing files (Gerber and drill files) that a PCB fabricator needs to build your board.

In this step, get ready to:
  • Transfer the schematic to the PCB Editor and set up board dimensions and design rules.
  • Route power and signal traces with proper widths and add a ground plane.
  • Run DRC, add silkscreen labels, and export Gerber and drill files for fabrication.
Transfer the schematic and set up the board

The PCB Editor needs your schematic data (component footprints, net connections) before you can start placing anything. KiCad can pull this directly from the schematic in one step.

  • In the KiCad PCB Editor, import your schematic data by clicking Tools in the top menu bar.
  • Click Update PCB from Schematic.
  • In the dialog that appears, click Update PCB to confirm the import.
  • Close the dialog. All your component footprints now appear in a cluster on the canvas, connected by thin lines (the ratsnest) showing which pads need to be connected.

What is the ratsnest?

The ratsnest is a set of thin lines showing the shortest path between pads that need to be connected by copper traces. As you place and route components, these lines disappear because the connections become real copper.

Next, you need to define the board size and the manufacturing rules your PCB fabricator expects.

  • Open the Board Setup dialog by clicking File then Board Setup.
  • In the Board Editor Layers section, confirm you have a 2-layer stackup (F.Cu and B.Cu enabled).
  • Navigate to Design Rules then Constraints.
  • Set Minimum track width to 0.25mm.
  • Set Minimum clearance to 0.2mm.
  • Click OK to save the board setup.

Now draw the board outline to define the physical size of your PCB.

  • Select the Edge.Cuts layer from the layer selector on the right side of the editor.
  • Use the Draw Rectangle tool from the right toolbar to draw a board outline approximately 25mm x 20mm.
  • You can type exact coordinates by pressing N to set precise dimensions after placing the first corner.

With the board outline in place, arrange your components inside it. Placement order matters for power electronics.

  • Place IC1 (the TPS561208, SOT-23-6 footprint) near the centre of the board.
  • Place C1, C2 (10 µF input caps) and C3 (0.1 µF decoupling) as close as possible to the VIN pin of IC1.
  • Place C4 (0.1 µF bootstrap cap) close to the BST and SW pins.
  • Place L1 (2.2 µH inductor) close to the SW pin, on the output side.
  • Place C5, C6 (22 µF output caps) close to where VOUT exits the inductor.
  • Place R1 (54.9 kΩ) and R2 (10 kΩ) for the feedback divider near the FB pin.
  • Place J1 (input connector) and J2 (output connector) at opposite edges of the board.

Why does placement order matter?

In a buck converter, the path from VIN through the high-side FET, low-side FET, and back through the input capacitors carries fast-changing current (high di/dt). The smaller the physical area this loop encloses, the less electromagnetic interference your board radiates.

Placing input capacitors close to the VIN and GND pins of the IC minimises this switching loop area. This is the single most important layout rule for any switching regulator.

Save your board by pressing Cmd+S (macOS) or Ctrl+S (Windows). Your ratsnest lines should now be short and relatively untangled.

Components not appearing after import?

If the canvas is empty after running Update PCB from Schematic, make sure you clicked Update PCB in the dialog (not just Close). Also check that your schematic has footprints assigned to every symbol. Help me troubleshoot the Update PCB from Schematic import.

Route the power path and add a ground plane

With components placed, you now need to connect them with copper traces. Power nets (VIN, SW, VOUT) carry up to 1A and need wider traces than signal nets.

  • Select the Route Tracks tool from the right toolbar (or press X).
  • Before routing, set your track width for power nets. In the top toolbar, change the track width to 0.5mm (for VIN and VOUT) or up to 1.0mm where space allows.
  • Route the VIN net from J1 through C1/C2/C3 to the VIN pin of IC1. Use the widest trace that fits.
  • Route the SW net from IC1's SW pin to L1. Keep this trace short and the copper area small to reduce EMI.
  • Route VOUT from L1 through C5/C6 to J2. Use 0.5mm or wider traces.
  • Route the feedback network (R1 and R2 to the FB pin) with thin traces (the default 0.25mm is fine). Keep these traces away from the SW node and inductor L1 to avoid noise coupling.
  • Route the BST net from C4 to the BST pin of IC1.

Why keep the SW node small?

The SW node is the noisiest point in a buck converter. It swings rapidly between VIN and ground at 580 kHz. Any copper connected to SW acts as an antenna radiating EMI. Keep the trace short and the copper area minimal.

Now add a solid ground plane on the bottom copper layer. This provides a low-impedance return path for all currents and helps with thermal dissipation.

  • Select the B.Cu (back copper) layer from the layer selector.
  • Click Add Filled Zone from the right toolbar.
  • In the zone properties dialog, set the net to GND.
  • Click OK, then draw the zone over the entire board outline by clicking each corner. Double-click to close the zone.
  • Press B to fill the zone. The entire bottom layer should now flood with copper connected to GND.

Finally, add vias to connect the top-side ground pads to the bottom ground plane.

  • For each ground pad on the top layer that is not directly connected to the ground plane, place a via nearby. Click the Add Via tool, click near the GND pad, and route a short trace from the pad to the via.
  • Place at least one via near IC1's GND pad, one near C1/C2's ground connections, and one near C5/C6's ground connections.
  • Save your board.

Why multiple ground vias?

Each via has a small amount of inductance. By using multiple vias distributed around the board, you provide a lower-impedance path to the ground plane. This is especially important near the input capacitors where high-frequency switching currents return through ground.

Zone not filling correctly?

If pressing B does not fill the zone, make sure your board outline is a closed shape on the Edge.Cuts layer. The zone fill uses the board outline as a boundary. Also check that you assigned the zone to the GND net (not "no net"). Help me debug my ground plane zone fill.

Run DRC, add silkscreen, and export fabrication files

Before sending your board to a fabricator, you need to verify there are no design rule violations, add readable labels, and generate the manufacturing files.

  • Run the Design Rule Check by clicking Inspect in the top menu bar.
  • Click Design Rules Checker.
  • In the DRC dialog, click Run DRC.
  • Resolve all errors and warnings. Common issues include clearance violations (move components apart), unconnected nets (add missing traces or vias), and unrouted connections shown as ratsnest lines.
  • Re-run DRC until you see zero violations. Close the DRC window.

What does DRC check?

DRC looks for design mistakes like copper regions with insufficient clearance, tracks that are too narrow, shorted nets, and mismatches between your schematic and the board layout. Fixing all DRC errors before manufacturing prevents expensive board respins.

Now add silkscreen text so you can identify the board and its connections after manufacturing.

  • Select the F.Silkscreen layer from the layer selector.
  • Use the Add Text tool from the right toolbar.
  • Add the board name BUCK-5V1A and version v1.0 in a visible area on the board.
  • Add polarity markers (+ and -) near J1 and J2 so you know which terminal is positive and which is ground.
  • Save your board.

Open the 3D Viewer to visually inspect your board before generating manufacturing files.

  • Click View in the top menu bar, then click 3D Viewer.
  • Rotate the board to check that components do not overlap, the board outline is correct, and silkscreen labels are readable.
  • Close the 3D Viewer when you are satisfied.

Finally, generate the Gerber and drill files that the PCB fabricator needs.

  • Click File in the top menu bar.
  • Click Plot.
  • In the Output directory field, type gerbers/ so all files go into a subfolder.
  • Confirm the plot format is set to Gerber.
  • Ensure these layers are checked: F.Cu, B.Cu, F.Silkscreen, B.Silkscreen, F.Mask, B.Mask, and Edge.Cuts.
  • Click Plot to generate the Gerber files.
  • Click Generate Drill Files at the bottom of the dialog.
  • In the drill file dialog, click Generate Drill File to create the .drl file.
  • Close the Plot dialog.

Verify that the gerbers/ folder was created inside your project directory.

  • In Finder (macOS) or File Explorer (Windows), navigate to your buck-converter-5v1a project folder.
  • Open the gerbers/ subfolder. You should see .gbr files for each layer and a .drl drill file.

What are Gerber files?

Gerber files are the industry-standard format for describing each layer of a PCB. Each .gbr file contains vector instructions for one copper, mask, or silkscreen layer. The drill file (.drl) tells the fabricator where to drill holes for through-hole components and vias.

Together, these files are everything a PCB fab house like JLCPCB or PCBWay needs to manufacture your board.

Missing layers in the Plot dialog?

If you do not see F.Silkscreen or B.Mask in the layer list, make sure those layers are enabled in Board Setup. Go to File then Board Setup, check that all required layers are ticked, and return to the Plot dialog. Help me figure out why layers are missing from my Gerber export.

Your PCB layout is complete and ready for manufacturing. Next up, you will order the boards, assemble your components, and test the converter on the bench.

Fabricate, Assemble, and Test

Your design is complete. You have a DRC-clean PCB layout, a verified simulation, and Gerber files ready to send to a factory.

Now it's time to turn those digital files into a physical circuit board. In this step, you'll order your boards from a PCB fabrication house, hand-solder every component, and validate your converter with real bench measurements.

In this step, get ready to:
  • Order your PCBs and components from a fabrication house and distributor.
  • Assemble the board using drag soldering and SMD hand-soldering techniques.
  • Power up, test, and document your converter's performance.
Order PCBs and components

PCB fabrication houses take your Gerber files and manufacture physical circuit boards from them. You'll upload the files you exported in the previous step and configure the board specifications to match your design.

  • Open your browser and navigate to jlcpcb.com (or pcbway.com as an alternative).
  • Create an account and log in.
  • Click Order Now or Instant Quote on the homepage.
  • Compress your gerbers/ folder into a single .zip file containing all Gerber and drill files.
  • Upload the .zip file. The system will automatically detect your board dimensions and layer count.
  • Use the Gerber Viewer to verify the preview matches your KiCad design.
  • Configure the board specifications: set Layers to 2, Thickness to 1.6mm, Surface Finish to HASL, and Quantity to 5 (minimum order).
  • Click Save to Cart, proceed to checkout, enter your shipping address, and complete payment.

Why order 5 boards?

Most PCB fabrication houses have a minimum order of 5 boards. The extras are useful for practising your soldering technique or giving spares to classmates. The cost difference between 1 and 5 boards is negligible.

While waiting for your boards to arrive (typically 1-2 weeks including shipping), order all components from your BOM.csv using DigiKey, Mouser, or LCSC.

  • Open BOM.csv and use the distributor part numbers to find each component.
  • Order at least 2-3 extra of each passive component (resistors and capacitors). They are inexpensive and easy to lose.
  • Gather your soldering tools: a temperature-controlled soldering iron with a fine tip, 0.5mm leaded solder, flux (pen or paste), tweezers, and a magnifying glass or microscope.

Leaded solder for beginners

Leaded solder (63/37 tin-lead) melts at a lower temperature and flows more easily than lead-free alternatives. It is significantly easier to work with for your first SMD project. Always wash your hands after soldering and work in a ventilated area.

Board preview doesn't match your design?

Check that your .zip contains both the Gerber files and the drill file (buck-converter-5v1a.drl) in the same archive. Missing drill files cause the viewer to show no holes. Also confirm you included the Edge.Cuts.gbr file for the board outline.

Help me troubleshoot my Gerber upload

Assemble the PCB

Once your boards and components arrive, it's time to solder. The TPS561208 in its SOT-23-6 package has only 6 pins and relatively wide spacing, making it approachable for hand soldering using the drag soldering technique.

  • Set your soldering iron to approximately 350°C.
  • Start with IC1 (the TPS561208). Apply flux to the SOT-23-6 pads on the PCB.
  • Align the IC with its pin 1 indicator matching the silkscreen dot on your board.
  • Tack one corner pin by melting a small amount of solder on a single pad and sliding the IC into position with tweezers.
  • Once aligned, tack the opposite corner pin to hold the IC firmly in place.
  • Apply flux along the remaining pins, then use the drag soldering technique: load a small bead of solder on your iron tip and drag it steadily across the pins. Surface tension causes the solder to wet each pin individually without bridging.

What is drag soldering?

Drag soldering uses flux and surface tension to solder multiple SMD pins in a single pass. You drag a bead of molten solder across a row of leads. The flux prevents the solder from bridging across the solder mask between pins, depositing an even amount on each lead.

If bridges form between pins, apply fresh flux to the bridge and touch it with a clean iron tip. The excess solder will wick away. For stubborn bridges, use desoldering braid (solder wick) to absorb the excess.

After IC1 is soldered, work through the remaining components from smallest to largest.

  • Solder the 0603 passives: R1 (54.9 kΩ), R2 (10 kΩ), and the bootstrap capacitor C4 (0.1 µF). For each part, tin one pad, slide the component in with tweezers, then solder the other end.
  • Solder the 1206 capacitors: input caps C2 and C3 (10 µF), output caps C5 and C6 (22 µF).
  • Solder the inductor L1 (2.2 µH shielded drum core).
  • Solder the input and output connectors J1 and J2.
  • Inspect every joint under magnification. Look for solder bridges (unwanted connections between adjacent pins), cold joints (dull, grainy appearance), and insufficient solder (the pad is visible through the joint).

Seeing solder bridges?

Apply fresh flux to the bridged area. Clean your iron tip, then drag it across the bridge. The excess solder will wick onto the tip. If that doesn't work, press a piece of solder wick (desoldering braid) on top of the bridge and heat from above. The braid absorbs the excess solder cleanly.

Help me fix solder bridges on my SMD components

Power up and test your converter

A systematic power-up procedure protects your board and power supply from damage if something is shorted. You will test incrementally, starting with no power and working up to full load.

  • Perform a final visual inspection. Look for any remaining solder bridges, components placed backwards, or missing parts.
  • Set your multimeter to resistance mode. Measure between VIN and GND on the input connector. The reading should not be near zero ohms. A near-zero reading indicates a short circuit that must be found and fixed before applying power.
  • Set your bench power supply to 12V with a current limit of 100 mA.
  • Connect the power supply to J1 (input connector), observing correct polarity.
  • Measure the output voltage across J2 with your multimeter. The target is 5.0V ± 2% (between 4.9V and 5.1V).
  • Gradually increase your load. Connect a 10 Ω resistor across the output (this draws 0.5A), then a 5 Ω resistor (1A). Raise the current limit on your supply accordingly.
  • Measure the output voltage under the 1A load. It should remain within the 5.0V ± 2% target.
  • If you have an oscilloscope, measure the output ripple voltage. The target is less than 50 mV peak-to-peak.
  • Calculate efficiency: measure input current and input voltage, then output voltage across the load. Efficiency = (VOUT × IOUT) / (VIN × IIN) × 100%.

Why start with a 100 mA current limit?

If there is a short on your board, a current-limited supply will simply drop its voltage rather than pushing destructive current through the fault. This protects both your components and your power supply. Once you confirm the output voltage is correct at low current, it is safe to increase the load.

Record all measurements in a test report document. Create a file called test_report.md in your project folder with the following structure:

# Test Report: Buck Converter 5V/1A

## Visual Inspection
- All joints inspected under magnification: PASS / FAIL
- No solder bridges detected: PASS / FAIL
- All components present and correctly oriented: PASS / FAIL

## Pre-Power Checks
- VIN to GND resistance: ___ Ω (should not be near zero)

## Output Voltage
- No load: ___ V (target: 5.0V ± 2%)
- 0.5A load: ___ V
- 1.0A load: ___ V (target: 5.0V ± 2%)

## Output Ripple
- Ripple at 1A load: ___ mV p-p (target: < 50 mV)

## Load Regulation
- Regulation = (V_no_load - V_full_load) / V_no_load × 100% = ___%

## Efficiency
- VIN: ___ V, IIN: ___ A
- VOUT: ___ V, IOUT: ___ A
- Efficiency = (VOUT × IOUT) / (VIN × IIN) × 100% = ___%

## Notes
- Any anomalies or observations during testing.

What does this document capture?

  • The visual inspection section records that you checked for assembly defects before powering up.
  • The output voltage section documents steady-state performance at different loads.
  • The efficiency calculation proves your converter performs well under real operating conditions.
  • This document becomes part of your portfolio alongside your schematic and layout screenshots.
  • Fill in test_report.md with your actual measurements as you run each test.
  • Take photos of your assembled board and your bench test setup for inclusion in your portfolio.

Finally, create a GitHub repository to house your complete project documentation.

  • Create a new repository on GitHub named buck-converter-5v1a.
  • Add all project files: the KiCad project (.kicad_pro, .kicad_sch, .kicad_pcb), the LTspice simulation file (buck_converter_sim.asc), the gerbers/ folder, BOM.csv, simulation_screenshots/, test_report.md, and a README.md.
  • Write a README.md that documents your full design process: requirements, component selection rationale, simulation results summary, schematic overview, PCB layout decisions, fabrication details, assembly notes, and test results.

Output voltage is wrong or zero?

If VOUT is 0V, check that the EN (enable) pin is connected to VIN either directly or through a resistor. An unconnected EN pin disables the converter.

If VOUT is higher or lower than expected, double-check R1 and R2 values with your multimeter. Swapped or incorrect feedback resistors are the most common cause of wrong output voltage.

Help me debug my buck converter output voltage

Your buck converter is alive and validated. You've taken a power electronics design from simulation through to working hardware. Next up, you'll extend this project with a USB charger output and power-good LED indicator.

Secret mission

USB Charger Output with Power-Good LED

Your buck converter works, but it sits on your bench as a bare board with test leads. What if it could actually charge your phone? In this secret mission, you'll add a USB Type-A output connector and a power-good LED indicator to transform your 5V/1A converter into a functional USB charger.

Clean Up Your Resources

Clean Up Your Resources

This project runs entirely on local software and physical hardware. There are no cloud resources, subscriptions, or ongoing costs to worry about.

Resources you used:

  • buck-converter-5v1a KiCad project folder (schematic, PCB layout, Gerbers, BOM, test report, simulation files).
  • KiCad 9 (installed application).
  • LTspice (installed application).
  • Assembled PCBs (physical hardware).

Keep everything running

No action needed. Choose this if you want to keep iterating on your design or use it as a reference for future projects.

  • Your assembled PCBs are physical hardware you own. Keep them in your portfolio and bring them to interviews as a tangible demonstration of your skills.
  • The spare PCBs from your order can be used to practice soldering techniques or given to classmates.
  • KiCad and LTspice are both free with no licensing costs. They take minimal disk space and are useful for future electronics projects.
  • Your project files, simulation screenshots, and test report make excellent GitHub portfolio material for job applications.

Pause - I'll come back to this later

There is nothing to pause. KiCad and LTspice have no background processes or services running. Your project files sit quietly on disk until you open them again.

  • If you want to free up disk space temporarily, you can compress your project folder into a zip archive and delete the uncompressed version.
  • Your Gerber files can always be regenerated from the KiCad project if needed.

Delete - I don't want to use this again

Remove all project files and optionally uninstall the design tools.

  • Delete your project folder by running the following command in Terminal (replace the path with wherever you saved the project):

macOS

rm -rf ~/Desktop/buck-converter-5v1a

Windows

rmdir /s /q %USERPROFILE%\Desktop\buck-converter-5v1a
  • To uninstall KiCad on macOS, open Finder, go to the Applications folder, and drag KiCad to the Trash. On Windows, go to Settings > Apps > Apps & features and uninstall KiCad from there.
  • To uninstall LTspice on macOS, open Finder, go to the Applications folder, and drag LTspice to the Trash. On Windows, go to Settings > Apps > Apps & features and uninstall LTspice from there.
  • Your physical PCBs can be recycled through an electronics waste (e-waste) facility if you no longer want them. Check your local council for drop-off locations.

That's a Wrap!

That's a Wrap!

You've designed, simulated, fabricated, and tested a real DC-DC converter from scratch. From a blank schematic to a working PCB on your bench, you now own the full power electronics design workflow.

Here's what you learned:

  • Designed a synchronous buck converter meeting a real specification (12V to 5V, 1A) and simulated it in LTspice to verify output voltage, ripple, and transient response before committing to hardware.
  • Captured a professional schematic in KiCad and laid out a 2-layer PCB with power electronics best practices including minimised switching loops, a solid ground plane, and proper component placement.
  • Generated Gerber files, ordered boards from a PCB fab house, assembled SMD components by hand, and validated the board with systematic power-up testing and load measurements.
  • Added a USB charger output with a power-good LED indicator, transforming the converter into a practical USB charging device that meets the USB 2.0 voltage specification.

Ready to quiz yourself?