# 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:

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

# 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.

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

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

# 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

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

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
CD4020BNSR	IC BINARY COUNTER 14-BIT 16SO	Texas Instruments	0_ic_logic	0_package_SO:SOIC-16_3.9x9.9mm_P1.27mm	296-CD4020BNSRCT-ND
CD4060BM96	IC BINARY COUNTER 14-BIT 16SOIC	Texas Instruments	0_ic_logic	0_package_SO:SOIC-16_3.9x9.9mm_P1.27mm	296-31513-1-ND
CD4514BM96	IC DECODER/DEMUX 1X4:16 24-SOIC	Texas Instruments	0_ic_logic	0_package_SO:SOIC-24W_7.5x15.4mm_P1.27mm	296-31529-1-ND
MC74HC04ADG	IC INVERTER 6CH 1-INP 14SOIC	onsemi	0_ic_logic	0_package_SO:SOIC-14_3.9x8.7mm_P1.27mm	MC74HC04ADGOS-ND
MC74HC32ADR2G	IC GATE OR 4CH 2-INP 14SOIC	-	0_ic_logic	0_package_SO:SOIC-14_3.9x8.7mm_P1.27mm	MC74HC32ADR2GOSCT-ND
SN74HC08DR	IC GATE AND 4CH 2-INP 14SOIC	Texas Instruments	0_ic_logic	0_package_SO:SOIC-14_3.9x8.7mm_P1.27mm	296-1191-1-ND
SN74HC138PWR	IC DECODER/DEMUX 1X3:8 16-TSSOP	Texas Instruments	0_ic_logic	0_package_SO:TSSOP-16_4.4x5mm_P0.65mm	296-8228-1-ND
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
SN74HC373DWR	8-bit Latch, 3-state outputs	Texas Instruments	0_ic_logic	0_package_SO:SOIC-20W_7.5x12.8mm_P1.27mm	296-1200-1-ND
SN74HC42DR	IC DECODER 1 X 4:10 16-SOIC	Texas Instruments	0_ic_logic	0_package_SO:SOIC-16_3.9x9.9mm_P1.27mm	296-8331-1-ND
ABS07-32.768KHZ-T	Two pin crystal	Abracon LLC	0_passive	Crystal:Crystal_SMD_3215-2Pin_3.2x1...	535-9542-1-ND

11 components — auto-generated 2026-03-09

Projects Using This Library

Project	Repo
Nixie Tube Clock	git.lokislair.com/aidanbrzezinski/Nixie_Tube_Clock

README.md

AidanBrzezinski KiCad Library

Table of Contents

Cloning a Project That Uses This Library