398 lines
13 KiB
Markdown
398 lines
13 KiB
Markdown
# AidanBrzezinski KiCad Library
|
|
|
|
Personal KiCad component library. Used as a git submodule in all projects.
|
|
|
|
---
|
|
|
|
## Table of Contents
|
|
|
|
- [Cloning a Project That Uses This Library](#cloning-a-project-that-uses-this-library)
|
|
- [Adding This Library to a New Project](#adding-this-library-to-a-new-project)
|
|
- [Best Practices](#best-practices)
|
|
- [Updating the Library Inside a Project](#updating-the-library-inside-a-project)
|
|
- [Adding Components to the Library](#adding-components-to-the-library)
|
|
- [Naming Conventions](#naming-conventions)
|
|
- [Symbol Field Reference](#symbol-field-reference)
|
|
- [Reference Designator Prefixes](#reference-designator-prefixes)
|
|
- [Value Field Conventions](#value-field-conventions)
|
|
- [Library Structure](#library-structure)
|
|
- [Component Index](#component-index)
|
|
- [Projects Using This Library](#projects-using-this-library)
|
|
|
|
---
|
|
|
|
## Cloning a Project That Uses This Library
|
|
|
|
The library is a submodule — it does not download automatically with a plain clone.
|
|
|
|
```bash
|
|
# Clone and initialise submodule in one step
|
|
git clone --recurse-submodules https://git.lokislair.com/aidanbrzezinski/YourProject
|
|
|
|
# Or if you already cloned without it
|
|
git submodule update --init --recursive
|
|
```
|
|
|
|
To never think about this again, set this globally on your machine:
|
|
|
|
```bash
|
|
git config --global submodule.recurse true
|
|
```
|
|
|
|
After that, `git pull` and `git clone` always include submodule updates automatically.
|
|
|
|
> **If KiCad prompts about missing libraries on open:** the submodule was not
|
|
> initialised. Run `git submodule update --init --recursive` and reopen the project.
|
|
|
|
---
|
|
|
|
## Adding This Library to a New Project
|
|
|
|
```bash
|
|
# From your project root
|
|
git submodule add https://git.lokislair.com/aidanbrzezinski/KiCad_Library lib/shared
|
|
|
|
# Copy the library table files into the project root
|
|
cp lib/shared/sym-lib-table ./sym-lib-table
|
|
cp lib/shared/fp-lib-table ./fp-lib-table
|
|
|
|
# Commit everything
|
|
git add .gitmodules lib/shared sym-lib-table fp-lib-table
|
|
git commit -m "lib: add shared KiCad library as submodule"
|
|
git push
|
|
```
|
|
|
|
KiCad reads `sym-lib-table` and `fp-lib-table` from the project root automatically.
|
|
These files must live in the **project root** — not inside `lib/shared`.
|
|
Always use `${KIPRJMOD}` in paths, never an absolute path.
|
|
`${KIPRJMOD}` resolves to the project root on any machine regardless of OS or
|
|
directory structure, keeping the repo portable.
|
|
|
|
---
|
|
|
|
## Best Practices
|
|
|
|
**Never modify the symbol drawing for standard parts.**
|
|
When copying from KiCad's global library, only change fields — never move pins,
|
|
resize the body, or change pin length. This keeps visual consistency across
|
|
every schematic that uses the library.
|
|
|
|
**Always use the full MPN as the symbol name.**
|
|
`SN74HC193DR` not `SN74HC193` or `74HC193`. The package suffix matters —
|
|
it determines the footprint and is what gets ordered from Digikey.
|
|
|
|
**One component per commit where possible.**
|
|
Makes git history readable and makes it easy to revert a bad footprint
|
|
without affecting anything else.
|
|
|
|
**Push library commit before updating the project pointer.**
|
|
If you update the pointer before pushing, other machines get a broken
|
|
submodule reference that cannot be resolved.
|
|
|
|
**Verify custom footprints against the physical part before committing.**
|
|
Draw from the datasheet first. When parts arrive, check with calipers.
|
|
A pad spacing error costs a full board respin.
|
|
|
|
**Re-copy table files when library categories are added.**
|
|
If `sym-lib-table` or `fp-lib-table` is updated in the library (new category added),
|
|
re-copy them into your project root and commit. See [Updating the Library](#updating-the-library-inside-a-project).
|
|
|
|
**Never register this library globally in KiCad.**
|
|
Global registration uses absolute paths that break on other machines.
|
|
Always use project-level table files with `${KIPRJMOD}`.
|
|
|
|
---
|
|
|
|
## Updating the Library Inside a Project
|
|
|
|
The submodule is pinned to a specific commit and never updates automatically.
|
|
This is intentional — library changes cannot silently break an existing project.
|
|
|
|
### Pull library updates into your project
|
|
|
|
```bash
|
|
cd lib/shared
|
|
git pull origin main
|
|
cd ../..
|
|
git add lib/shared
|
|
git commit -m "lib: update shared library to latest"
|
|
git push
|
|
```
|
|
|
|
### Make library changes from within a project
|
|
|
|
```bash
|
|
# The submodule directory IS the library repo
|
|
cd lib/shared
|
|
|
|
# Make changes — add symbol, footprint etc
|
|
git add symbols/0_ic_logic.kicad_sym
|
|
git commit -m "lib: add SN74HC193DR"
|
|
git push origin main # pushes to the LIBRARY repo
|
|
|
|
# Return to project root and update the pointer
|
|
cd ../..
|
|
git add lib/shared
|
|
git commit -m "lib: update shared library pointer"
|
|
git push # pushes to the PROJECT repo
|
|
```
|
|
|
|
Two commits are produced — one in the library repo with the actual change,
|
|
one in the project repo advancing the pinned commit pointer.
|
|
|
|
### Check which library commit your project is using
|
|
|
|
```bash
|
|
git submodule status
|
|
# a3f8c2d lib/shared (heads/main)
|
|
# ^ this hash is the exact library commit your project is pinned to
|
|
```
|
|
|
|
### Re-sync table files after library structure changes
|
|
|
|
```bash
|
|
cp lib/shared/sym-lib-table ./sym-lib-table
|
|
cp lib/shared/fp-lib-table ./fp-lib-table
|
|
git add sym-lib-table fp-lib-table
|
|
git commit -m "lib: sync library table files"
|
|
```
|
|
|
|
---
|
|
|
|
## Adding Components to the Library
|
|
|
|
### Standard components (exist in KiCad global library)
|
|
|
|
```
|
|
1. KiCad → Symbol Editor
|
|
2. Find chip in global 74xx / 4xxx / Device library
|
|
3. Right click → Copy
|
|
4. Navigate to your 0_xx library → Right click → Paste
|
|
5. Right click → Rename to full MPN including package suffix
|
|
e.g. SN74HC193 → SN74HC193DR
|
|
6. Double click → Edit Symbol Fields:
|
|
|
|
Value: SN74HC193DR
|
|
Footprint: 0_package_SO:SOIC-16_3.9x9.9mm_P1.27mm
|
|
Datasheet: https://www.ti.com/lit/ds/symlink/sn74hc193.pdf
|
|
MPN: SN74HC193DR
|
|
Digikey_PN: 296-1191-1-ND
|
|
Manufacturer: Texas Instruments
|
|
Library_Source: KiCad 8.0 global 74xx lib
|
|
|
|
7. File → Save
|
|
8. Commit and push from inside lib/shared:
|
|
|
|
git add symbols/0_ic_logic.kicad_sym
|
|
git commit -m "lib: add SN74HC193DR"
|
|
git push origin main
|
|
|
|
9. Update submodule pointer in the project repo:
|
|
|
|
cd ../..
|
|
git add lib/shared
|
|
git commit -m "lib: update shared library pointer"
|
|
git push
|
|
```
|
|
|
|
### Custom components (not in KiCad global library)
|
|
|
|
```
|
|
1. Check SnapEDA: snapeda.com/search/?q=PARTNUMBER
|
|
2. If found:
|
|
→ Download KiCad package (symbol + footprint + 3D model)
|
|
→ Import symbol → clean up to match KiCad style:
|
|
pin length 100mil, text size 1.27mm
|
|
inputs on left, outputs on right, power top/bottom
|
|
→ Copy .kicad_mod → footprints/0_custom.pretty/
|
|
→ Copy .step → 3d_models/
|
|
3. If not found — draw from datasheet:
|
|
→ Symbol from pin table
|
|
→ Footprint from mechanical drawing
|
|
→ Verify footprint with calipers on physical part before PCB layout
|
|
4. Set all fields and commit same as above
|
|
```
|
|
|
|
### Commit message format
|
|
|
|
```
|
|
lib: add SN74HC193DR
|
|
lib: add SN74HC193DR SN74HC163DR
|
|
lib: fix HV5622PG footprint pad spacing
|
|
lib: update SMBJ15A Digikey PN
|
|
lib: add 0_ic_analog category
|
|
```
|
|
|
|
---
|
|
|
|
## Naming Conventions
|
|
|
|
### Symbol names
|
|
Always use the full MPN including package suffix:
|
|
```
|
|
SN74HC193DR ✓ includes package suffix (SOIC-16)
|
|
SN74HC193 ✗ ambiguous — which package?
|
|
74HC193 ✗ missing manufacturer prefix
|
|
```
|
|
|
|
### Footprint file names
|
|
```
|
|
# Standard packages — KiCad convention
|
|
SOIC-16_3.9x9.9mm_P1.27mm.kicad_mod
|
|
|
|
# Custom parts — MPN + package
|
|
HV5622PG_DIP44.kicad_mod
|
|
|
|
# Custom parts with no single MPN — function + mounting type
|
|
IN14_NixieTube_THT.kicad_mod
|
|
EC11_Encoder_THT.kicad_mod
|
|
```
|
|
|
|
### 3D model file names
|
|
Match the footprint name exactly:
|
|
```
|
|
HV5622PG_DIP44.step
|
|
IN14_NixieTube_THT.step
|
|
```
|
|
|
|
### Datasheet URLs
|
|
Always link directly to the manufacturer PDF, not a product page:
|
|
```
|
|
# Texas Instruments
|
|
https://www.ti.com/lit/ds/symlink/sn74hc193.pdf
|
|
|
|
# ON Semiconductor
|
|
https://www.onsemi.com/pdf/datasheet/mc74hc193a-d.pdf
|
|
|
|
# Microchip
|
|
https://ww1.microchip.com/downloads/en/DeviceDoc/HV5622.pdf
|
|
```
|
|
|
|
TI pattern: `https://www.ti.com/lit/ds/symlink/LOWERCASE_MPN.pdf`
|
|
|
|
---
|
|
|
|
## Symbol Field Reference
|
|
|
|
Every symbol must have these fields populated before committing:
|
|
|
|
| Field | Example | Notes |
|
|
|---|---|---|
|
|
| Value | `SN74HC193DR` | Full MPN including package suffix |
|
|
| Footprint | `0_package_SO:SOIC-16_3.9x9.9mm_P1.27mm` | Library nickname : footprint name |
|
|
| Datasheet | `https://www.ti.com/lit/ds/symlink/sn74hc193.pdf` | Direct PDF link — manufacturer only |
|
|
| MPN | `SN74HC193DR` | Exact manufacturer part number |
|
|
| Digikey_PN | `296-1191-1-ND` | Digikey PN at time of addition |
|
|
| Manufacturer | `Texas Instruments` | Manufacturer name |
|
|
| Library_Source | `KiCad 8.0 global 74xx lib` | Where the symbol drawing came from |
|
|
|
|
---
|
|
|
|
## Reference Designator Prefixes
|
|
|
|
| Component | Prefix |
|
|
|---|---|
|
|
| All ICs (logic, power, driver, MCU) | U |
|
|
| Resistors | R |
|
|
| Capacitors | C |
|
|
| Inductors | L |
|
|
| Diodes | D |
|
|
| Crystals | Y |
|
|
| Connectors | J |
|
|
| Switches / buttons | SW |
|
|
| Transistors / FETs | Q |
|
|
| Test points | TP |
|
|
| Nixie tubes | NX |
|
|
| Ferrite beads | FB |
|
|
|
|
---
|
|
|
|
## Value Field Conventions
|
|
|
|
| Component | Value field contains |
|
|
|---|---|
|
|
| ICs | Full MPN — `SN74HC193DR` |
|
|
| Resistors | `10k`, `4.7k`, `100R` |
|
|
| Capacitors | `100nF 50V`, `10uF 25V` |
|
|
| Crystals | `32.768kHz` |
|
|
| Diodes | MPN — `SMBJ15A` |
|
|
| Connectors | Function — `12V_IN` |
|
|
| Buttons | Function — `SW_CYCLE` |
|
|
|
|
---
|
|
|
|
## Library Structure
|
|
|
|
```
|
|
AidanBrzezinski_KiCad_Library/
|
|
│
|
|
├── .github/
|
|
│ ├── workflows/
|
|
│ │ └── update_component_index.yml # Auto-updates Component Index in README
|
|
│ └── scripts/
|
|
│ └── update_component_index.py # Parser script — run locally or in CI
|
|
│
|
|
├── symbols/ # KiCad symbol libraries (.kicad_sym)
|
|
│ ├── 0_ic_logic.kicad_sym # 74xx 4xxx general logic
|
|
│ ├── 0_ic_mcu.kicad_sym # Microcontrollers
|
|
│ ├── 0_ic_driver.kicad_sym # Motor HV gate LED drivers
|
|
│ ├── 0_ic_power.kicad_sym # Regulators converters
|
|
│ ├── 0_ic_analog.kicad_sym # Op-amps comparators ADCs DACs
|
|
│ ├── 0_ic_rf.kicad_sym # RF ICs transceivers
|
|
│ ├── 0_ic_interface.kicad_sym # CAN RS-422 USB interface ICs
|
|
│ ├── 0_passive.kicad_sym # R C L crystals
|
|
│ ├── 0_connector.kicad_sym # All connectors
|
|
│ └── 0_discrete.kicad_sym # Diodes transistors buttons encoders
|
|
│
|
|
├── footprints/ # Footprint libraries (.pretty folders)
|
|
│ │ # Standard packages: populated as needed
|
|
│ │ # or reference KiCad global via ${KICAD8_FOOTPRINT_DIR}
|
|
│ ├── 0_package_SO.pretty/ # SOIC SOP SSOP
|
|
│ ├── 0_package_SOT_TO_SMD.pretty/ # SOT-23 TO-252 TO-263
|
|
│ ├── 0_package_QFP.pretty/ # QFP LQFP
|
|
│ ├── 0_package_DFN_QFN.pretty/ # DFN QFN
|
|
│ ├── 0_package_SON.pretty/ # SON
|
|
│ ├── 0_capacitor_smd.pretty/ # SMD capacitors
|
|
│ ├── 0_resistor_smd.pretty/ # SMD resistors
|
|
│ ├── 0_inductor_smd.pretty/ # SMD inductors
|
|
│ ├── 0_diode_smd.pretty/ # SMD diodes
|
|
│ ├── 0_led_smd.pretty/ # SMD LEDs
|
|
│ ├── 0_transistor_fet.pretty/ # Transistors FETs
|
|
│ ├── 0_connector.pretty/ # Connectors
|
|
│ ├── 0_switch_button.pretty/ # Switches buttons
|
|
│ ├── 0_switching_regulator.pretty/ # Regulator modules
|
|
│ ├── 0_interface_uart.pretty/ # Interface connectors
|
|
│ ├── 0_testpoint.pretty/ # Test points
|
|
│ ├── 0_fiducials.pretty/ # Fiducials
|
|
│ ├── 0_pad.pretty/ # Bare pads
|
|
│ ├── 0_net_tie.pretty/ # Net ties
|
|
│ ├── 0_mousebites.pretty/ # Panel breakaway tabs
|
|
│ └── 0_custom.pretty/ # Non-standard parts: IN-14 HV5622 NCH6300HV EC11
|
|
│
|
|
├── 3d_models/ # STEP and WRL 3D models (flat)
|
|
│ └── *.step / *.wrl # Named by MPN or footprint name
|
|
│
|
|
├── sym-lib-table # ← COPY TO PROJECT ROOT
|
|
├── fp-lib-table # ← COPY TO PROJECT ROOT
|
|
├── CHANGELOG.md
|
|
├── LICENSE
|
|
└── README.md
|
|
```
|
|
|
|
---
|
|
|
|
## Component Index
|
|
|
|
| MPN | Description | Manufacturer | Symbol Library | Footprint | Digikey PN |
|
|
|---|---|---|---|---|---|
|
|
| SN74HC193DR | Synchronous 4-bit Up/Down (2 clk) counter | Texas Instruments | 0_ic_logic | 0_package_SO:SOIC-16_3.9x9.9mm_P1.27mm | 296-41634-1-ND |
|
|
|
|
*1 components — auto-generated 2026-03-08*
|
|
|
|
|
|
## Projects Using This Library
|
|
|
|
| Project | Repo |
|
|
|---|---|
|
|
| Nixie Tube Clock | git.lokislair.com/aidanbrzezinski/Nixie_Tube_Clock |
|