Personal Kicad Library Convention (KLC)

Personal Kicad library conventions for symbol libraries. Inspired by the official KiCad Library Convention (KLC) but adapted for a fully specified component library.

1. Scope

These conventions apply to all symbol libraries prefixed with MyLib_. Every symbol in these libraries should be fully specified. It represents one exact purchasable component with a pre-assigned footprint, datasheet, and distributor information.

2. Library Naming

Libraries are named by function using the format:

MyLib_<Function>

Use singular nouns and CamelCase for multi-word functions.

Library Name	Contents
`MyLib_Capacitor`	All capacitor types
`MyLib_Resistor`	Resistors, including arrays
`MyLib_Inductor`	Inductors, ferrite beads
`MyLib_Diode`	Diodes, TVS, Zener, Schottky, LEDs
`MyLib_IC_Power`	Voltage regulators, charge ICs
`MyLib_MCU`	Microcontrollers
`MyLib_Connector`	Various connectors (FFC, Pin Headers)
`MyLib_Sensor`	Temperature, IMU, pressure, etc.
`MyLib_Oscillator`	Crystals, oscillators, resonators

3. Symbol Naming

Symbols follow the format:

<RefDes>_<Value>_<Package>_<Manufacturer>_<MPN>

3.1 Field Definitions

Field	Description	Examples
`<RefDes>`	Standard reference designator prefix	`C`, `R`, `L`, `U`, `D`, `Q`, `J`, `Y`
`<Value>`	Human-readable electrical value or function	`100nF`, `10k`, `3.3V-LDO`
`<Package>`	Package identifier	`0402`, `0603`, `SOT-23`, `SOIC-8`, `QFN-32`
`<Manufacturer>`	Manufacturer name	`Murata`, `TI`, `ST`, `Nexperia`
`<MPN>`	Manufacturer part number	`GRM155R71C104KA88`

3.2 Examples

Symbol Name	Library
`C_100nF_0402_Murata_GRM155R71C104KA88`	`MyLib_Capacitor`
`R_10k_0603_Yageo_RC0603FR-0710KL`	`MyLib_Resistor`
`U_3.3V-LDO_SOT-23-5_TI_TLV75533PDBV`	`MyLib_IC_Power`
`U_STM32F103C8_LQFP-48_ST_STM32F103C8T6`	`MyLib_MCU`
`D_Red_0603_Wurth_150060RS75000`	`MyLib_LED`
`J_USB-C_Amphenol_12401610E4-2A`	`MyLib_Connector`

3.3 Special Cases

ICs where the value is essentially the part number: Use a short functional description as the value instead of repeating the MPN. E.g. U_3.3V-LDO_... rather than U_TLV75533_..._TI_TLV75533PDBV.
Connectors: Value can describe the function or pin count, e.g. J_USB-C_..., J_2x5-SWD_....

4. Required Symbol Fields

Every symbol must contain the following fields.

4.1 Standard KiCad Fields

Field	Visibility	Content
`Reference`	Visible	Standard RefDes (`C`, `R`, `U`, `D`, `Q`, `J`, `L`, etc.)
`Value`	Visible	Symbol name (matches the full symbol name from Section 3)
`Footprint`	Hidden	Full footprint path, e.g. `Capacitor_SMD:C_0402_1005Metric`
`Datasheet`	Hidden	URL to the manufacturer datasheet (PDF link preferred)

4.2 Custom Fields

Field	Visibility	Content
`Manufacturer`	Hidden	Manufacturer name, e.g. `Murata`, `Texas Instruments`
`Manufacturer Part Number`	Hidden	Exact orderable MPN, e.g. `GRM155R71C104KA88J`
`Distributor Link 1`	Hidden	URL to primary distributor product page
`Distributor 1 Part Number`	Hidden	Primary distributor’s SKU, e.g. `490-16434-1-ND` (Digi-Key)
`Distributor Link 2`	Hidden	URL to secondary distributor product page
`Distributor 2 Part Number`	Hidden	Secondary distributor’s SKU, e.g. `81-GRM155R71C104KA8J` (Mouser)

4.3 Field Notes

The Manufacturer Part Number field contains the full, exact orderable MPN.
Distributor fields enable one-click ordering and BOM export to purchasing tools.
If only one distributor source is known, leave Distributor Link 2 and Distributor 2 Part Number as ~.
All custom fields are hidden to keep the schematic clean.
If possible download a PDF of the datasheet and host it on your own server/keep it locally.

5. Footprint Association

Every symbol must have a default footprint assigned in the Footprint field.
If the same component exists in multiple packages, create a separate symbol for each package.

6. General Rules

6.1 Characters

Only use: A-Z, a-z, 0-9, _, -, ., ,, +
No spaces in symbol or library names.

6.2 Symbol Graphics

Whenever possible derive symbols from the Kicad library.
When creation of a custom symbol or footprint is necessary, follow the official KLC for pin placement, outline style, and text sizes.
Consider upstreaming the generic variant of the component to the Kicad library.

6.3 Adding a New Part — Checklist

Before a symbol is considered complete, verify:

Symbol name follows <RefDes>_<Value>_<Package>_<Manufacturer>_<MPN> format
Symbol is placed in the correct MyLib_<Function> library
Reference field is correct and visible
Value field matches symbol name and is visible
Footprint field points to a valid footprint and is hidden
Datasheet field contains a working URL and is hidden
Manufacturer field is filled and hidden
Manufacturer Part Number field is filled and hidden
Distributor Link 1 and Distributor 1 Part Number are filled and hidden
Distributor Link 2 and Distributor 2 Part Number are filled (or set to ~) and hidden
Footprint filters are set
Symbol has been visually checked in the symbol editor

7. Revision History

Version	Date	Notes
1.0	2026-03-14	Initial release

1. Scope#

2. Library Naming#

3. Symbol Naming#

3.1 Field Definitions#

3.2 Examples#

3.3 Special Cases#

4. Required Symbol Fields#

4.1 Standard KiCad Fields#

4.2 Custom Fields#

4.3 Field Notes#

5. Footprint Association#

6. General Rules#

6.1 Characters#

6.2 Symbol Graphics#

6.3 Adding a New Part — Checklist#

7. Revision History#