KiCad Template Project

Overview

The Leafony template for KiCad lets you start designing an expansion leaf with the Leafony bus contacts and board outline already configured. It includes a schematic, PCB, dedicated symbol and footprint libraries, layer configuration, and design rules.

The setup and usage instructions on this page are based on the KiCad template README on GitHub (Japanese).

Development environment

• KiCad 10.0.x
• KiCad’s standard symbol and footprint libraries

Supported version

The included schematics, PCB, and footprints are saved in KiCad 10.0 format. The previous requirement of “KiCad 5.0.0 or later” does not apply to the current files. KiCad 9 and earlier are not supported.

When starting KiCad for the first time, choose the option to use its standard libraries. If your system provides the libraries as separate packages, as on some Linux distributions, install those packages as well. Power symbols in the schematic use the standard power library.

Download

On GitHub - leafony/cad-template, select Code → Download ZIP and extract the archive. If you use Git, you can download the repository with this command:

git clone https://github.com/leafony/cad-template.git

Download the entire folder, since the project also needs its libraries and other referenced files. In the paths below, replace cad-template with the actual folder where you cloned the repository or extracted the ZIP archive.

Main files

The following files and folders are inside cad-template/KiCad/Leafony_Template/.

Path	Purpose
Leafony_Template.kicad_pro	Project settings, design rules, and net classes
Leafony_Template.kicad_sch	Schematic with the Leafony bus, power connections, and signal labels
Leafony_Template.kicad_pcb	PCB with the board outline, contacts, vias, and copper zone keepouts
lib/Leafony.kicad_sym	Leafony Bus symbol
lib/Leafony.pretty/	CN_F29_B29 footprint
sym-lib-table	Project-specific symbol library table; empty as distributed
fp-lib-table	Project-specific footprint library table; Leafony is already registered
meta/	Template name, description, icon, and preview image

Register lib/Leafony.kicad_sym as the symbol library, rather than the legacy files leafony_template-cache.lib, lib/Leafony.dcm, or lib/Leafony.bak. The .kicad_prl and fp-info-cache files contain personal settings and cached data; they are not libraries to register.

Usage

Register the user template

1. Launch the KiCad project manager.
2. Open Preferences → Configure Paths…. Menu names may vary with your OS and display language.
3. Set KICAD_USER_TEMPLATE_DIR to the absolute path of the KiCad folder in the downloaded repository.
4. Save the settings. If the template does not appear in the list, restart KiCad.

OS	Example setting
Windows	C:/Users/your-name/Documents/cad-template/KiCad
macOS	/Users/your-name/Documents/cad-template/KiCad
Linux	/home/your-name/cad-template/KiCad

This variable must point to the parent folder containing Leafony_Template. Check that Leafony_Template/meta/info.html exists under the configured folder.

If you already use another user template folder, you can keep that setting and copy the entire Leafony_Template folder into it.

Create a new project

1. In the project manager, select File → New Project….
2. Select Leafony Leaf from the template list. Filter the list to user templates if needed.
3. Click OK, then choose a working folder and a new project name, such as my_leaf.
4. Open the generated my_leaf.kicad_pro, then launch the schematic and PCB editors from the project manager.

The template files are copied into the new project, and the main files are renamed to match the project name. The lib folder and library tables are also copied. Save the new project in a different location from the original template folder.

To inspect the template, you can open Leafony_Template/Leafony_Template.kicad_pro directly. To design your own leaf, edit the newly created project.

Configure the symbol library

The template’s sym-lib-table, copied into the new project, is empty as distributed. Placed symbols are also stored in the schematic, but you must register the library to add or reference symbols from it.

1. Open the schematic editor from the project manager.
2. Open Preferences → Manage Symbol Libraries….
3. Select Project Specific Libraries.
4. Use the option to add an existing library and select lib/Leafony.kicad_sym inside your new project.
5. Set the entries to the following values, enable the library, and save.

Field	Value
Nickname	Leafony
Library path	${KIPRJMOD}/lib/Leafony.kicad_sym
Library format	KiCad

${KIPRJMOD} is the current project folder, set automatically by KiCad. You do not need to add or change it in the path settings.

Check that Leafony:Leafony Bus appears in the symbol chooser. If you are using the existing CN1, you do not need to place another symbol just to check the library.

Check the footprint library

The footprint library is already registered in fp-lib-table, so no additional setup is normally needed. In the PCB editor, open Preferences → Manage Footprint Libraries… and check the project-specific libraries.

Field	Value
Nickname	Leafony
Library path	${KIPRJMOD}/lib/Leafony.pretty
Library format	KiCad

The library is configured correctly if Leafony:CN_F29_B29 appears. If you register it again, select the Leafony.pretty folder, not an individual .kicad_mod file.

When moving or sharing the project with another PC, copy the entire project, including the lib folder and library tables, to preserve the relative references using ${KIPRJMOD}.

Start designing

Template defaults

The values below are the settings in the included files. Check the layer configuration, manufacturing constraints, and net classes in Board Setup, and compare them with your manufacturer’s requirements.

Item	Default value
Board outline	Maximum Edge.Cuts dimensions: 23 × 20 mm. The connector side is 20 mm wide, with extensions on both sides of the board
Copper layers	4 layers: F.Cu / In1.Cu / In2.Cu / B.Cu
Board thickness	0.8 mm
Bus contacts	CN1, with 29 contacts on each side (F1–F29 and B1–B29)
Mounting holes	Two non-plated holes, 2.05 mm in diameter
Minimum track width and minimum clearance	0.1016 mm
Track width for the Default net class	0.127 mm
Via diameter / drill diameter for the Default net class	0.56 mm / 0.30 mm

Copper zone keepouts are configured around the connector. Use the PCB data as the reference for the actual board outline, contact positions, and hole positions.

Edit the schematic and PCB

1. Check the pin assignments of the leaves you will use, then add components and wiring to the schematic. Verify the Leafony bus contact numbers and existing signal names as you connect them.
2. Assign footprints to the added components and run the schematic’s electrical rules check (ERC).
3. Select Tools → Update PCB from Schematic… to apply the changes to the PCB.
4. Check the contact and mounting hole positions, as well as possible component interference with other leaves, then place the components and route the board.
5. Refill the copper zones and run the design rules check (DRC) to check for unconnected items and manufacturing rule violations.
6. Export the Gerber and drill files, and check them against your manufacturer’s requirements.

See the Custom Leaf Development resources for pin assignments and I2C addresses.

Troubleshooting

Symptom	What to check
Leafony Leaf does not appear in the template list	Check that KICAD_USER_TEMPLATE_DIR points to the parent folder of Leafony_Template, with Leafony_Template/meta/info.html underneath it. Reopen the list or restart KiCad.
KiCad reports that the file format is too new	Check that you are opening the files with KiCad 10.0.x.
The Leafony symbol library cannot be found	Register Leafony in the new project’s symbol library table. It is not registered in the distributed table.
Leafony:CN_F29_B29 cannot be found	Check that the project contains lib/Leafony.pretty and fp-lib-table, and that the nickname and path match the settings above.
Standard symbols such as power cannot be found	Check that KiCad’s standard libraries are installed and enabled in the global library table.
Libraries cannot be found after moving to another PC	Copy the lib folder as well, and check that library paths use ${KIPRJMOD} instead of absolute paths from the original PC.

License

The template is released under the MIT license.