Skip to the content
2 layers45 × 35 mmBuck5v, the printed circuit board in 3D

A 2-layer synchronous buck converter board built around the Texas Instruments TPS54202. Input is 9 to 24 V, output is 5 V at up to 2 A, with a switching frequency of about 500 kHz.

Size
45 × 35 mm
Copper layers
2
Thickness
1.6 mm
Parts
20
Nets
8
Pads
40
Tracks, vias
38, 50
Pours
2
Routed
Yes
KiCad
KiCad 10.0 (file 20260206)
Created
18 Oct 2026
Updated
19 Oct 2026

Overview

Buck5v is an open-source printed circuit board by Karthikeya2005, from the Karthikeya2005/buck5v repository on GitHub, published under the MIT licence. It is a 2-layer board of 45 × 35 mm with 20 parts on 8 nets, routed with 38 tracks and 50 vias.

It is built around the TPS54202DDCR and SS34. Its parts include 7 capacitors, 4 resistors, 2 connectors, 1 IC and 1 diode.

Main components

2

README

README.md

buck5v: 12 V to 5 V, 2 A Buck Converter (KiCad 10)

A 2-layer synchronous buck converter board built around the Texas Instruments TPS54202. Input is 9 to 24 V, output is 5 V at up to 2 A, with a switching frequency of about 500 kHz.

Status: designed and checked in software only. The board has not been fabricated, assembled or measured. Every figure below is a calculation from the datasheet, not a bench result. Part sourcing (stock, LCSC numbers) was not verified either.

I built this to learn power-supply design end to end: choosing the IC, calculating each component, wiring the schematic, laying out the board around the switching loop, and checking it with ERC and DRC. I checked the datasheet values and reviewed the schematic, layout and DRC results myself.

Schematic PCB layout 3D view

Specification

ParameterValue
Input voltage9 to 24 V (IC accepts 4.5 to 28 V)
Output voltage5 V (about 5.03 V typical)
Output current2 A
Switching frequency500 kHz typical (390 to 630 kHz)
TopologySynchronous buck, integrated FETs
Board2 layers, 45 x 35 mm
ProtectionSeries Schottky for reverse polarity, EN divider as undervoltage lockout

Design

IC: TPS54202DDCR

4.5 to 28 V input, 2 A, internal high-side and low-side FETs, so no external catch diode is needed. Datasheet values I used: feedback voltage VFB = 0.596 V (0.581 to 0.611 V), switching frequency 500 kHz, low-side current limit up to 4.3 A.

Output voltage

Vout = VFB x (1 + R1 / R2) = 0.596 x (1 + 102 k / 13.7 k) = 5.03 V typical. Over the VFB tolerance the output spans 4.91 to 5.16 V. Both resistors are standard 1% values.

Inductor

L = 15 uH (Sunlord MWSA1004S-150MT: 45 mOhm DCR max, Isat 5.6 A taken conservatively from the datasheet).

VinDuty cycleRipple current (p-p)Peak current at 2 A load
9 V0.560.30 A2.15 A
12 V0.420.39 A2.19 A
24 V0.210.53 A2.26 A

Ripple current = Vout x (1 - D) / (L x f). Peak current stays well below both the inductor's 5.6 A saturation current and the IC's 4.3 A maximum low-side limit.

Capacitors

RefValueRole
C1, C210 uF 50 V X7R (1210)Bulk input
C3100 nF 50 V X7R (0603)High-frequency input decoupling, placed at the VIN pin
C4100 nF 50 V X7R (0603)Bootstrap, BOOT to SW
C5, C622 uF 25 V X7R (1210)Output
C775 pF C0G (0603), not populatedOptional feed-forward across R1

Ceramic capacitance falls with DC bias, so the effective output capacitance at 5 V is lower than 44 uF. Output ripple depends mostly on ESR and layout, so it has to be measured on a real board.

Enable divider (undervoltage lockout)

R4 = 511 k from VIN to EN, R5 = 105 k from EN to GND. With the datasheet EN rising threshold of 1.21 V typical (1.28 V max), the converter starts at about 7.1 V (7.5 V worst case) at the IC's VIN node. EN sees about 1.5 V at 9 V in and about 4.1 V at 24 V in. Check this against the datasheet's absolute maximum rating for EN before building.

Reverse-polarity protection

D1 is an SS34 Schottky in series with the input. It costs roughly 0.5 V and about 0.6 W at 9 V in and 2 A out. A P-channel MOSFET would waste less power but needs extra parts.

Bill of materials

RefValueFootprint
U1TPS54202DDCRTSOT-23-6 (hand-solder variant)
L115 uH, MWSA1004S-150MTSunlord MWSA1004S
D1SS34 SchottkySMA
C1, C210 uF 50 V X7R1210
C3, C4100 nF 50 V X7R0603
C5, C622 uF 25 V X7R1210
C775 pF C0G (DNP)0603
R1102 k 1%0603
R213.7 k 1%0603
R4511 k 1%0603
R5105 k 1%0603
J1, J22-pin screw terminal5.00 mm pitch
TP1 to TP4Test points: VIN, VOUT, SW, GND1.5 mm pad

Ordering would need a fresh sourcing pass. Several part numbers (including the inductor) were not confirmed in stock, and the 5.00 mm terminal block should be matched to a real part.

Layout notes

  • The input capacitors sit at the IC's VIN pin. Because SW is between VIN and GND on the 6-pin package, the 100 nF cap's ground return is about 10 mm, so the loop is tight on the VIN side only.
  • SW copper is short (about 13 mm in total including the test point). The boot-cap branch off the SW node is about 6 mm, longer than ideal.
  • VIN and SW are necked down to 0.65 mm for the first 1.3 to 1.5 mm at the 0.95 mm pin pitch so the 0.25 mm clearance rule holds. Other power traces are 1.0 mm or wider.
  • The feedback divider sits near the FB pin, away from SW and L1.
  • The bottom layer is a GND plane with stitching vias. The EN trace runs on the bottom layer, short and clear of the switching nodes.
  • The TSOT-23-6 has no thermal pad, so heat leaves through the GND pin copper. Thermal performance has not been verified.

Verification

CheckResult
ERC0 errors (PWR_FLAG symbols added to VIN, GND and +5V)
DRC0 errors, 0 unconnected items at the last run
DRC warningsMostly stitching vias flagged "not connected on one layer" (the top-layer GND zone only covers a small patch near the IC) and a few silkscreen overlaps
Schematic to board syncNo differences

Known limitations

  • Not built or measured. No efficiency, ripple, thermal or EMI data.
  • The top-layer GND pour should cover the whole board. As it stands, the stitching vias outside the patch near U1 only connect to the bottom plane.
  • Component sourcing and the 5.00 mm terminal-block part are unverified.
  • Ripple and thermal estimates depend on real capacitor ESR and copper area, which this design does not confirm.

Test plan (if built)

TestSetupWhat to look for
Power-upBench supply at 12 V, current limit 0.2 A, no load5.0 V on TP2, no oscillation or smoke
Output accuracy9, 12, 24 V in, no load and 2 A loadOutput within about +/-3% of 5 V
Efficiency0.1, 0.25, 0.5, 1, 1.5, 2 A at 9, 12, 24 VMeasure Vin and Iin at the board terminals, Vout and Iout at the load
Output rippleScope on TP2 with spring ground at TP4, 20 MHz bandwidthRipple in mV, compare with the estimate
SW waveformScope on TP3Duty cycle, ringing, frequency near 500 kHz
Load step0.2 A to 2 AOvershoot and recovery
Thermal2 A for 10 minutes, thermal camera or thermocoupleIC and inductor temperature rise
Start-up thresholdSlowly raise Vin from 0Converter starts near 7 to 7.6 V

Repository layout

text
buck5v.kicad_pro        KiCad project
buck5v.kicad_sch        Schematic
buck5v.kicad_pcb        PCB layout
buck5v.kicad_sym        Project symbol library (TPS54202)
sym-lib-table           Library table for the project symbol
docs/                   Images of the schematic, board and 3D view
fab/                    Gerber files, drill files and BOM (CSV)
buck5v-gerbers.zip      The fab/ folder zipped, ready to upload to a board house

Open buck5v.kicad_pro in KiCad 10 or newer.

Tools

KiCad 10. Datasheet values were checked by hand against the TI TPS54202 and Sunlord MWSA-S datasheets.

License

MIT. See LICENSE. There is no warranty, and nobody has independently reviewed this design. Have it reviewed before building it or using it in anything that matters.

Parts

20
QtyValueFootprintReferences
2100nF 50V X7RCapacitor_SMD:C_0603_1608MetricC3, C4
210uF 50V X7RCapacitor_SMD:C_1210_3225MetricC1, C2
222uF 25V X7RCapacitor_SMD:C_1210_3225MetricC5, C6
1102k 1%Resistor_SMD:R_0603_1608MetricR1
1105k 1%Resistor_SMD:R_0603_1608MetricR5
113.7k 1%Resistor_SMD:R_0603_1608MetricR2
115uH MWSA1004S-150MTInductor_SMD:L_Sunlord_MWSA1004SL1
1511k 1%Resistor_SMD:R_0603_1608MetricR4
175pF C0G DNPCapacitor_SMD:C_0603_1608MetricC7
1GNDTestPoint:TestPoint_Pad_D1.5mmTP4
1SS34Diode_SMD:D_SMAD1
1SWTestPoint:TestPoint_Pad_D1.5mmTP3
1TPS54202DDCRPackage_TO_SOT_SMD:TSOT-23-6_HandSolderingU1
1VINTestPoint:TestPoint_Pad_D1.5mmTP1
1VIN 9-24VTerminalBlock:TerminalBlock_MaiXu_MX126-5.0-02P_1x02_P5.00mmJ1
1VOUTTestPoint:TestPoint_Pad_D1.5mmTP2
1VOUT 5V 2ATerminalBlock:TerminalBlock_MaiXu_MX126-5.0-02P_1x02_P5.00mmJ2

Similar boards

  • 4 layers21.7 × 89.8 mmEuroPlatvorm, the printed circuit board in 3D

    EuroPlatvorm

    nanassound/eurorack-nanassound

    Eurorack modules of Nanas Sound

    34 parts27
  • 4 layers95 × 58 mmEsp32Tap, the printed circuit board in 3D

    Esp32Tap

    scottmsilver/treddy

    Controlling my procor-9.3x treadmill

    94 parts2
  • 4 layers128 × 55 mmCluster2HDMI, the printed circuit board in 3D

    Cluster2HDMI

    vkar9898/Cluster2HDMI

    A project dedicated to utilising a 7 inch LCD panel as a standalone monitor via a HDMI-parallel RGB converter and a Pico 2 fitted on a custom PCB

    96 parts2MIT
  • 2 layers60 × 47.5 mm86 BOX PANEL, the printed circuit board in 3D

    86 BOX PANEL

    yaozong1/86BOX_PCB

    86_BOX PCB

    48 parts1
  • 2 layers60 × 46 mmCardboard bot, the printed circuit board in 3D

    Cardboard bot

    ColumbiaGadgetWorks/cardboard-bot-v2

    60 × 46 mm, 2-layer, 2 oz copper, for a 2S or 3S LiPo on a screw terminal. JLCPCB assembles the SMD parts on the top side; CGW hand-solders the through-hole parts. Nothing goes on the back.

    67 parts
  • 2 layers104 × 66 mmVallox rs485-controller, the printed circuit board in 3D

    Vallox rs485-controller

    Miroeilola/vallox-rs485-controller

    Replacement control panel for legacy Vallox SE ventilation units. Vallox DIGIT RS-485 protocol, bus-powered, ESP32, Home Assistant.

    65 parts
  • 4 layers70 × 45 mmEmanresu G431, the printed circuit board in 3D

    Emanresu G431

    EmanresuEmanreztuneb/SimpleFOC_G431_Motordriver

    A motordriver based in STM's G431 Drone ESC.

    112 parts3

Questions

How big is the Buck5v PCB?

It measures 45 × 35 mm and has 2 copper layers, 1.6 mm thick.

What parts does the Buck5v use?

20 parts, built around the TPS54202DDCR and SS34. The full list of its parts is on this page, with links to each part's symbol and footprint where PCBKit's library has them.

Where can I download the Buck5v KiCad files?

From the Karthikeya2005/buck5v repository on GitHub, at the commit this page was made from: the board is buck5v.kicad_pcb and its schematic buck5v.kicad_sch. PCBKit opens the board in the browser, with nothing to install.

Can I use the Buck5v design in my own project?

Its repository publishes it under the MIT licence: you may reuse it on that licence's terms (keep the author's notice, and for a copyleft licence share your changes alike).