Skip to main content
Guides

Exporting a KiCad Library

Overview​

tscircuit allows you to export your circuit designs as a KiCad Library. Unlike the KiCad Project export (which creates a complete project file), the KiCad Library export creates reusable components that can be imported into any KiCad project.

The exported library includes:

  • Symbol Library (.kicad_sym) - Schematic symbols for all components
  • Footprint Library (.pretty folder) - PCB footprints for all components
  • 3D Models (.3dshapes folder) - 3D model files (STEP/WRL) referenced by footprints
  • Library Tables (fp-lib-table, sym-lib-table) - Configuration files for KiCad to locate the libraries

How to Export KiCad Library​

Using the Browser​

  1. Run tsci dev in your project directory to start the development server
  2. Navigate to File > Export > KiCad Library
  3. A zip file will be downloaded containing all library files

Using the CLI​

You can also export directly from the command line:

tsci export ./my-circuit.tsx -f kicad-library

This creates a directory in the same location as the input file:

my-circuit-kicad-library/
├── my-circuit.kicad_sym          # Symbol library
├── my-circuit.pretty/            # Footprint library
│   ├── resistor.kicad_mod
│   ├── capacitor.kicad_mod
│   └── ...
├── my-circuit.3dshapes/          # 3D models
│   └── component.step
├── fp-lib-table                  # Footprint library table
└── sym-lib-table                 # Symbol library table

What's Inside the Export​

Symbol Library (.kicad_sym)​

Contains schematic symbols for all components in your circuit. Each symbol includes:

  • Pin definitions with correct electrical types
  • Reference designator (e.g., R1, C1, U1)
  • Footprint association linking to the corresponding footprint

Footprint Library (.pretty folder)​

Contains PCB footprints for each unique component. Each .kicad_mod file includes:

  • Pad definitions (SMD or through-hole)
  • Silkscreen graphics
  • Courtyard outlines
  • 3D model references (pointing to the .3dshapes folder)

3D Models (.3dshapes folder)​

Contains STEP files for 3D visualization in KiCad's 3D viewer. These are automatically:

  • CLI: Copied from the source paths in your project
  • Browser: Fetched via HTTP and included in the zip

Library Tables​

Configuration files that tell KiCad where to find the libraries:

fp-lib-table - Footprint library configuration:

(fp_lib_table
  (lib (name my-circuit)(type KiCad)(uri ${KIPRJMOD}/my-circuit.pretty)(options "")(descr ""))
)

sym-lib-table - Symbol library configuration:

(sym_lib_table
  (lib (name my-circuit)(type KiCad)(uri ${KIPRJMOD}/my-circuit.kicad_sym)(options "")(descr ""))
)

Using the Library in KiCad​

  1. Extract/Copy the library to your KiCad project folder or a shared libraries location

  2. Add the library tables to your KiCad project:

    • Copy fp-lib-table and sym-lib-table to your project folder, OR
    • Merge the entries into your existing library tables

  3. Use the symbols and footprints in your KiCad schematic and PCB:

    • Symbols appear under the library name you exported
    • Footprints are automatically linked to symbols

Including 3D Models​

To include 3D models in your export, add a cadModel prop to your components:

<chip
  name="SW1"
  footprint="pushbutton"
  cadModel={
    <cadmodel
      modelUrl={stepUrl}
      rotationOffset={{ x: 0, y: 0, z: 270 }}
      positionOffset={{ x: 0.5, y: -0.3, z: 0 }}
    />
  }
/>

The 3D model will be:

  • Referenced in the footprint file with the correct path
  • Included in the .3dshapes folder of the export

Example​

Here's a complete example of a circuit with components that will be exported:

import stepUrl from "./switch.step"

circuit.add(
  <board width="20mm" height="20mm">
    <resistor name="R1" resistance="1k" footprint="0402" />
    <capacitor name="C1" capacitance="1uF" footprint="0603" />
    <chip
      name="SW1"
      footprint="pushbutton"
      cadModel={
        <cadmodel
          modelUrl={stepUrl}
          rotationOffset={{ x: 0, y: 0, z: 270 }}
        />
      }
    />
    <trace from=".R1 .pin2" to=".C1 .pin1" />
  </board>
)

Exporting this circuit will create a library with:

  • 3 symbols (resistor, capacitor, chip)
  • 3 footprints (resistor_0402, capacitor_0603, chip)
  • 1 3D model (switch.step)