Skip to the content
2 layers34.7 × 45.2 mmSD card, the printed circuit board in 3D

A minimal 3.3 V microSD card breakout board designed in KiCad for SPI communication with microcontrollers. Created as a hands-on PCB design project; schematic complete and ERC-clean, with layout, fabrication, and hardware testing still pending.

Size
34.7 × 45.2 mm
Copper layers
2
Thickness
1.6 mm
Parts
9
Nets
8
Pads
37
Tracks, vias
50, 3
Pours
2
Routed
Yes
KiCad
KiCad 10.0 (file 20260206)
Created
12 Jun 2026
Updated
16 Jun 2026

Overview

SD card is an open-source printed circuit board by isaacmatt, from the isaacmatt/SD_Card_Breakout_Board repository on GitHub. It is a 2-layer board of 34.7 × 45.2 mm with 9 parts on 8 nets, routed with 50 tracks and 3 vias.

Its parts include 5 resistors, 2 capacitors and 2 connectors. It belongs with the interfaces and adapters and microcontroller boards boards of this library.

README

README.md

microSD Card Breakout (SPI, 3.3 V)

A minimal microSD card breakout board for 3.3 V microcontrollers, exposing the card over a 1-bit SPI interface on a 0.1" header. Designed as a hands-on KiCad project with a clean, manufacturable layout.

Status: Schematic and PCB layout complete. ERC and DRC clean (0 violations, 0 unconnected). Not yet fabricated or tested — this is a design-stage project. Footprint assignment, layout, and manufacturing files are done; the board has not been ordered, assembled, or brought up.


Overview

This is a passive breakout: it routes a microSD connector to a pin header with the minimum support circuitry required for reliable operation, and nothing else. No onboard microcontroller, voltage regulator, level shifter, or USB. You supply 3.3 V from a host, jumper the SPI lines across, and talk to the card using a standard SD library on the host side.

The design deliberately targets the common denominator across 3.3 V hosts: SPI 1-bit mode . SDIO/4-bit is intentionally out of scope.

Features

  • microSD (TF) push-push connector with spring eject
  • SPI 1-bit interface broken out to a 1×8 0.1" header
  • Pull-ups on all data lines per the SD specification
  • Local decoupling (100 nF + 1 µF) at the connector's VDD pin
  • 2-layer board with ground pours on both layers, via-stitched
  • All passives 0603 (hand-solder friendly); designed for low-cost fab + assembly

Specifications

PropertyValue
InterfaceSPI, 1-bit
Logic / supply voltage3.3 V only (not 5 V tolerant )
Layers2 (signals on top, GND pours both layers)
ConnectorSHOU HAN TF PUSH, push-push, 8 contacts + grounded shell
Connector LCSC P/NC393941
Card detectionFirmware (no hardware detect switch — see below)
EDA toolKiCad 10

Supported hosts

HostSupportedNotes
Raspberry Pi Pico W (RP2040)✅ Direct3.3 V SPI host
nRF52840✅ Direct3.3 V SPI host
Arduino Uno (ATmega328P)⚠️ Not directly5 V logic — its SPI outputs would overdrive a 3.3 V card. Requires an external level shifter on SCK/MOSI/CS. Not included on this board.

microSD cards operate at 2.7–3.6 V and are not 5 V tolerant. Any 5 V-logic host requires level shifting on the host-driven lines (SCK, MOSI, CS). MISO returns 3.3 V, which a 5 V AVR reads as a valid logic high, so only the outbound lines need shifting.

Pinout

microSD contact → SPI mapping

The microSD pinout is standardized. In SPI mode:

ContactCard nameSPI roleOn-board support
1DAT2unused10 kΩ pull-up
2CD/DAT3CS10 kΩ pull-up
3CMDMOSI10 kΩ pull-up
4VDDpower100 nF + 1 µF decoupling
5CLKSCK—
6VSSground—
7DAT0MISO10 kΩ pull-up
8DAT1unused10 kΩ pull-up
shellshield—tied to GND

DAT1 and DAT2 are unused in SPI mode but are pulled high so the card does not float into an undefined state at power-up.

J2 header (1×8, 2.54 mm)

PinSignal
13V3
2GND
3CS
4SCK
5MOSI
6MISO
7GND
8GND

The header order was chosen to keep board routing clean; the two extra grounds improve the jumper-wire return path.

Card detection

The chosen connector has no mechanical card-detect switch — only the 8 SD contacts and a grounded shell. Card presence is therefore detected in firmware : attempt to initialize the card over SPI, and if it responds, a card is present. This is standard practice for SD breakouts and removes a dependency on an underdocumented mechanical feature.

Bill of Materials

RefValuePackageNotes
J1microSD connectorSMDSHOU HAN TF PUSH, LCSC C393941
J21×8 header2.54 mm THTHand-soldered after SMT assembly
C1100 nF0603Decoupling at VDD
C21 µF0603Bulk decoupling at VDD
R110 kΩ0603CS pull-up
R210 kΩ0603MOSI pull-up
R310 kΩ0603MISO pull-up
R410 kΩ0603DAT1 pull-up
R510 kΩ0603DAT2 pull-up

Design decisions & rationale

  • 3.3 V-only, passive breakout. Keeps the board simple and lets it work with any 3.3 V SPI host. Level shifting is treated as a host-side concern, not baked in.
  • SPI 1-bit mode. The common denominator across target hosts; also simplifies the breakout to CS/SCK/MOSI/MISO + power.
  • Pull-ups on all data lines. Per the SD physical-layer specification, including the unused DAT1/DAT2 so they don't float; CS is pulled high so it idles correctly.
  • Decoupling placed at the connector's VDD pin. SD cards have real current inrush; the 100 nF + 1 µF sit immediately at the power pin where they're effective.
  • Connector selected for availability. An active, in-stock, JLCPCB-assemblable part was prioritized over a "nicer" datasheet on an out-of-stock alternative — a manufacturability-driven choice.
  • Firmware card detection. Chosen over relying on a hardware switch the connector doesn't have.
  • Dual-layer GND pour, via-stitched. Grounds the connector shield, provides a low-impedance return, and ties both planes together.

Manufacturing notes

Intended fab/assembly flow (JLCPCB):

  1. Order bare PCBs + economic SMT assembly for the connector and 0603 passives.
  2. Leave the through-hole header (J2) off the assembly and hand-solder it afterward — it's the easiest part and avoids THT assembly fees.
  3. At the assembly stage, verify the connector's pad-1 orientation in the placement preview — connector rotation is the most common first-time assembly mistake.

The pull-up resistors and caps are all 0603 and the only THT part is the header, so the board is straightforward to assemble either by machine or by hand.

Not included / limitations

  • No level shifting — 3.3 V hosts only.
  • No ESD protection — see roadmap.
  • No mounting holes are electrically connected (the connector's holes are mechanical/NPTH).
  • Untested; no firmware/driver provided. Use a standard SPI SD library on the host (e.g. Arduino SD/SdFat, CircuitPython adafruit_sdcard, or the RP2040/nRF SDKs).

Roadmap (v2 ideas)

  • Add a low-capacitance ESD/TVS array at the connector contacts (e.g. USBLC6-2SC6 or a multi-channel low-cap array), placed before the pull-ups. Low capacitance matters so SPI edges aren't distorted.
  • Optional level-shifted variant (e.g. 74LVC125 buffer + 3.3 V LDO) to support 5 V hosts like the Arduino Uno directly.
  • Silkscreen the full header pinout next to J2 for at-a-glance jumpering.

Repository structure

text
.
├── microSD_breakout.kicad_pro     # KiCad project
├── microSD_breakout.kicad_sch     # Schematic
├── microSD_breakout.kicad_pcb     # PCB layout
├── easyeda2kicad.pretty/          # Imported connector footprint
├── easyeda2kicad.kicad_sym        # Imported connector symbol
├── fab/                           # Gerbers, BOM, CPL (when generated)
├── docs/                          # Schematic / PCB / 3D renders
└── README.md

Opening this project

The connector's symbol and footprint are bundled in this repository (easyeda2kicad.pretty/, easyeda2kicad.kicad_sym) so the project opens without external dependencies. The library tables reference them with the project-relative path variable ${KIPRJMOD}, so the paths resolve correctly on any machine after cloning.

If KiCad reports a missing footprint or symbol after cloning, check that the footprint and symbol library tables point to the in-repo copies (Preferences → Manage Footprint/Symbol Libraries) using ${KIPRJMOD}/easyeda2kicad.pretty and ${KIPRJMOD}/easyeda2kicad.kicad_sym.

Regenerating the connector footprint

The J1 footprint was imported from LCSC using easyeda2kicad. To regenerate it from scratch:

bash
pip install easyeda2kicad
easyeda2kicad --full --lcsc_id C393941

Then add the generated easyeda2kicad.pretty and easyeda2kicad.kicad_sym to your KiCad library tables. Using the EasyEDA/LCSC library this way ensures the footprint geometry matches JLCPCB's pick-and-place data for assembly.

Wiring example

Connect the J2 header to your host's SPI pins. The exact host GPIO numbers depend on your board — fill in your host's SPI bus:

J2 pinSignal→ Host
13V33.3 V
2GNDGND
3CSany GPIO used as chip-select
4SCKSPI clock
5MOSISPI MOSI / TX
6MISOSPI MISO / RX
7GNDGND
8GNDGND

License

MIT — choose and add a LICENSE file. MIT is a common default for open hardware projects; adapt as you prefer.

Author

isaac-m (@isaacmatt)


Built in KiCad as a from-scratch PCB design exercise: connector selection and lifecycle/stock checking, third-party footprint import and verification, schematic capture, layout, ground-plane routing, and manufacturing-file preparation.

Parts

9
QtyValueFootprintReferences
510kResistor_SMD:R_0603_1608MetricR1, R2, R3, R4, R5
1100nFCapacitor_SMD:C_0603_1608MetricC1
11uFCapacitor_SMD:C_0603_1608MetricC2
1Conn_01x08Connector_PinHeader_2.54mm:PinHeader_1x08_P2.54mm_VerticalJ2
1Micro_SD_Cardeasyeda2kicad:TF-SMD_TF-PUSHJ1

Similar boards

  • 2 layers103 × 30.5 mmTS Back Endcap, the printed circuit board in 3D

    TS Back Endcap

    EEVengers/ThunderScope

    ThunderScope GitHub Repo

    9 parts1.3kMIT
  • 2 layers31.8 × 47.6 mmNGC 38 connector, the printed circuit board in 3D

    NGC 38 connector

    rusefi/rusefi

    rusefi - GPL internal combustion engine control unit

    9 parts1.2k
  • 2 layers24 × 27.3 mmExpansion Card Retrofit, the printed circuit board in 3D

    Expansion Card Retrofit

    FrameworkComputer/ExpansionCards

    Reference designs and documentation to create Expansion Cards for the Framework Laptop

    9 parts1.1kCC-BY-4.0
  • 2 layers15.6 × 17.3 mmSKR Mini TFT Thermistor Board, the printed circuit board in 3D

    SKR Mini TFT Thermistor Board

    VoronDesign/Voron-Hardware

    Cool Hardware designed by the Voron Design group

    9 parts1.1kGPL-3.0
  • 2 layers39.1 × 49.5 mmLearnoliver, the printed circuit board in 3D

    Learnoliver

    hackclub/OnBoard

    💡 Join 1,000 teenagers and make your first PCB with a $100 grant!

    9 parts915
  • 2 layers17.4 × 16.9 mmToolhead, the printed circuit board in 3D

    Toolhead

    tanaes/whopping_Voron_mods

    9 parts787GPL-3.0
  • 2 layers9.8 × 108 mmExpander, the printed circuit board in 3D

    Expander

    wntrblm/Castor_and_Pollux

    A Juno-inspired dual oscillator

    9 parts587
  • 2 layersKeyboard after, the printed circuit board in 3D

    Keyboard after

    adamws/kicad-kbplacer

    KiCad plugin for automatic keyboard's key placement and routing

    9 parts547GPL-3.0

Questions

How big is the SD card PCB?

It measures 34.7 × 45.2 mm and has 2 copper layers, 1.6 mm thick.

What parts does the SD card use?

9 parts. 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 SD card KiCad files?

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

Can I use the SD card design in my own project?

Its repository states no licence, so its author keeps all rights: ask isaacmatt before reusing the design.