MIKILAB KiCad Library

Personal, self-contained KiCad library for MIKILAB hardware projects.

This directory is fully autonomous: it does not depend on kicad-personal-library or any other external directory. Every path used inside sym-lib-table, fp-lib-table and the footprint 3D model references is relative to this library (via ${KIPRJMOD}), so the whole folder can be moved, renamed, zipped, or synced to another machine without breaking anything.

Architecture

Every .kicad_sym file under symbols/ is an independent KiCad symbol library (there is deliberately no single monolithic MIKILAB.kicad_sym). Every .pretty directory under footprints/ is likewise an independent KiCad footprint library. This mirrors how the official KiCad libraries are structured and keeps components easy to find, diff, and maintain individually.

mikylab_kikad_library/
├── sym-lib-table         # registers every symbols/**/*.kicad_sym
├── fp-lib-table          # registers every footprints/**/*.pretty
├── symbols/<category>/<Name>.kicad_sym
├── footprints/<category>/<Name>.pretty/<Name>.kicad_mod
├── 3dmodels/<category>/<Name>.step
├── docs/                 # reference documentation (incl. upstream KiCad docs)
├── legacy/                # legacy .lib/.dcm sources kept for reference
├── scripts/               # import & check tooling (this README's §5, §6)
├── MANIFEST.csv           # full provenance/status log, one row per file
└── README.md

Categories in use: analog, audio, display, fpga_cpld, interface, logic, mechanical, memory, microcontrollers, other, power, rf.

Every symbol/footprint library is registered under a MIKILAB_<name> nickname, e.g. MIKILAB_TPS7A2012PDBVR, MIKILAB_TPS7A2018PDBVR, MIKILAB_Amplifier_Operational, MIKILAB_altera. Nicknames are derived automatically from the file/directory name and are guaranteed unique.

1. Installing the library

There are two ways to make this library available in KiCad. Which one you want depends on whether you use it in one project or in every project.

Option A -- one project only (no KiCad config changes)

sym-lib-table / fp-lib-table at the root of this repo use ${KIPRJMOD}, which KiCad automatically resolves to the currently open project's directory. So if a .kicad_pro project lives directly inside mikylab_kikad_library/ (or you copy these two table files into your project's directory), KiCad picks them up automatically -- no extra configuration needed. This is the setup check_library.py and the scripts/ tooling assume.

Option B -- available in every project (recommended for a personal library)

This is the practical setup for a library you want in every schematic you open, not just one project. Tested against the KiCad 10.0 install on this machine (/Applications/KiCad/KiCad.app, config at ~/Library/Preferences/kicad/10.0/).

1. Define an environment variable pointing at this library. KiCad → Preferences → Configure Paths... → add a new entry:

   • Name: MIKILAB
   • Path: /Users/michelebigi/Development/mikylab_kikad_library

2. Generate the "global" table variant (uses ${MIKILAB} instead of ${KIPRJMOD}; regenerate any time after adding components):

   python3 scripts/generate_global_tables.py
   

   This writes sym-lib-table.global and fp-lib-table.global at the library root.

3. Merge those into KiCad's global tables. The simplest way is to append their (lib ...) lines into your existing global tables (back them up first):

   cp ~/Library/Preferences/kicad/10.0/sym-lib-table ~/Library/Preferences/kicad/10.0/sym-lib-table.bak
   cp ~/Library/Preferences/kicad/10.0/fp-lib-table  ~/Library/Preferences/kicad/10.0/fp-lib-table.bak
   
   python3 - <<'EOF'
   import re
   from pathlib import Path
   
   kicad_dir = Path.home() / "Library/Preferences/kicad/10.0"
   lib_root = Path("/Users/michelebigi/Development/mikylab_kikad_library")
   
   for kind, global_file, generated in (
       ("sym_lib_table", "sym-lib-table", "sym-lib-table.global"),
       ("fp_lib_table", "fp-lib-table", "fp-lib-table.global"),
   ):
       target = kicad_dir / global_file
       new_libs = (lib_root / generated).read_text().splitlines()
       new_libs = [l for l in new_libs if l.strip().startswith("(lib")]
   
       text = target.read_text()
       # insert the new (lib ...) lines just before the final closing paren
       idx = text.rstrip().rfind(")")
       text = text.rstrip()[:idx] + "\n" + "\n".join(new_libs) + "\n" + text.rstrip()[idx:] + "\n"
       target.write_text(text)
       print(f"Merged {len(new_libs)} libraries into {target}")
   EOF
   

   (Or do it by hand: open both .global files and copy each (lib ...) line into the corresponding file under ~/Library/Preferences/kicad/10.0/, just before the final closing ).)

4. Restart KiCad. Every MIKILAB_* symbol and footprint library is now available in any project, resolved via ${MIKILAB}.

Known issue on this machine, to clean up before deleting kicad-personal-library: the current global sym-lib-table already has a handful of entries pointing directly at /Users/michelebigi/Development/kicad-personal-library/... with absolute paths (added before this library existed, e.g. libraries named ti, TPS63020DSJT). Once the MIKILAB_* libraries above are installed and working, remove those old absolute-path entries from ~/Library/Preferences/kicad/10.0/sym-lib-table -- otherwise you'll have duplicate/stale libraries, and deleting kicad-personal-library will leave KiCad with broken references. This library's own tables never contain absolute paths (verified by check_library.py and by grep -R "/Users/michelebigi"), so this cleanup is only about your existing global KiCad config, not about anything in this repo.

2. Using the symbols

In the schematic editor, symbols are available as MIKILAB_<LibraryName>:<SymbolName>, e.g. MIKILAB_TPS7A2012PDBVR:TPS7A2012PDBVR or MIKILAB_Amplifier_Operational:LM358.

3. Using the footprints

In the footprint assignment tool / PCB editor, footprints are available as MIKILAB_<LibraryName>:<FootprintName>, e.g. MIKILAB_SOT95P280X145_5N:SOT95P280X145-5N.

4. How 3D models are resolved

Footprints reference 3D models with ${KIPRJMOD}/3dmodels/<category>/<Name>.step, resolved relative to this library — portable by construction, no absolute paths anywhere.

Known gap (pre-existing, not introduced by this cleanup): a set of vendor-imported footprints (footprints/other/*.pretty and a few others — see check_library.py warnings) reference 3D models via ${KISBLIB}/..., an environment variable that is not defined by this library or by a stock KiCad install, and the corresponding 3D files were never present locally to begin with. These footprints are fully usable for schematic/PCB work (pads, courtyard, silkscreen are all correct and complete) — they simply won't show a 3D body until you either supply the matching STEP/WRL file and update the reference, or define KISBLIB in KiCad pointing at wherever you keep those vendor 3D models. run scripts/check_library.py lists every affected file.

Some IPC-generated footprints reference the standard KiCad 3D model library via ${KISYS3DMOD}, which is defined automatically by every KiCad installation — those resolve normally and need no action.

Special case — shared footprint, distinct 3D bodies: SOT95P280X145-5N is used by both MIKILAB_TPS7A2012PDBVR and MIKILAB_TPS7A2018PDBVR. The footprint itself was verified byte-identical between the two parts (SHA256 comparison showed the only difference was KiCad's internal tedit timestamp), so a single shared footprint library is used. Their 3D bodies are genuinely different STEP files, though (3dmodels/power/TPS7A2012PDBVR.step vs. .../TPS7A2018PDBVR.step), and a .kicad_mod can only carry one embedded (model ...) reference — so neither is embedded by default. If you want a 3D render for one of these parts, assign the STEP file manually per footprint instance (PCB editor → right-click footprint → Properties → 3D Models).

5. Adding a component

Simplest path — one command:

python3 scripts/add_component.py \
    --name TPS7A2018PDBVR \
    --symbol /path/to/TPS7A2018PDBVR.kicad_sym \
    --footprint /path/to/SOT95P280X145-5N.kicad_mod \
    --model /path/to/TPS7A2018PDBVR.step \
    --category power

--footprint and --model are optional — you can import a symbol-only component, or symbol+footprint without a 3D model. --category is optional too; it's auto-detected from --name using the same rules used throughout this library (falls back to other).

The importer:

• refuses to overwrite a component that already exists (by name), with a clear error and no changes made;
• deduplicates footprints by content (SHA256), not filename — if the footprint you're importing is byte-identical to one already in the library, the existing one is reused instead of creating a duplicate;
• if a different footprint happens to share a filename with an existing one, it is imported under a distinct, semantically-derived name and the collision is recorded in MANIFEST.csv;
• rewrites the symbol's Footprint property to point at the correct new MIKILAB_<lib>:<name> reference;
• links the 3D model into the footprint (unless the footprint was reused from an existing shared library — see §4's shared-footprint case);
• regenerates sym-lib-table and fp-lib-table from scratch by scanning the directory tree, so there is never more than one (version 7) entry and every library on disk is registered exactly once;
• appends a row per file to MANIFEST.csv (columns: type, source, destination, status, hash, notes; status is one of NEW, DUPLICATE, RENAMED_COLLISION, ERROR, UNCHANGED).

import_component.py is the same tool with a more explicit/verbose CLI — add_component.py just calls into it. For importing many components at once, lay them out one subdirectory per component and run:

python3 scripts/import_batch.py --source /path/to/batch_dir [--category power]

(subdirectory name = component --name; exactly one .kicad_sym per subdirectory required, footprint/model optional — same collision and lib-table rules as a single import, applied per component).

To import directly from a SnapEDA (SnapMagic Search) "Download KiCad" zip, without unzipping it by hand first:

python3 scripts/import_snapeda.py --zip ~/Downloads/PARTNUMBER.zip [--name ...] [--category ...]

It unzips to a temp directory, locates the .kicad_sym / .kicad_mod / 3D model inside by extension (SnapEDA's internal folder layout varies between downloads), and hands off to the same import_component.py core -- identical validation, collision handling, and lib-table regeneration as every other import path here.

6. Running the check

python3 scripts/check_library.py

Verifies: directory structure; symbol/footprint syntax and duplicates; real filename collisions (by content hash, not just name); 3D model reference validity and portability; sym-lib-table/fp-lib-table syntax, single (version 7), no missing/duplicate/unregistered entries; and symbol → footprint cross-references for every MIKILAB-owned library. Exits 0 (RESULT: OK) iff there are no errors. Warnings are pre-existing, documented, non-fatal gaps (see §4).

Note: many symbols mirrored from the official KiCad symbol libraries reference standard KiCad footprint libraries (e.g. Package_SO, RF_Module) by their upstream nickname — those are outside MIKILAB's scope (they ship with every KiCad install) and are not checked or reported as errors.

FSC-BT1035 (symbol only, hand-authored -- footprint still needed)

symbols/rf/FSC-BT1035.kicad_sym (Feasycom Bluetooth 5.2 dual-mode stereo audio module, Qualcomm QCC3056) was hand-authored from the official Feasycom datasheet Table 3-2 (Pin definition) -- all 52 pins, names and electrical types transcribed directly from that table and validated with kicad-cli sym export. No existing KiCad symbol for this part could be found publicly (SnapEDA blocks unauthenticated access; no GitHub project had one).

No footprint or 3D model is included. The datasheet's mechanical section (module 13 x 26.9 x 2.2mm, castellated LCC-52 package, 1.0mm pad pitch, antenna keep-out on one edge) has enough detail to build one, but extracting exact per-pad coordinates reliably from the PDF's dimensioned drawing (rather than a real coordinate table) was judged too error-prone to commit blind -- a wrong castellated-pad footprint could produce an unfabricatable board without anyone noticing until parts don't line up. A working footprint for this exact part does exist (fabricated, per the gerbers) in manvalan/DigiRadio's EasyEDA project, but its pad geometry is embedded in EasyEDA's proprietary JSON format, which wasn't reverse-engineered here. Import a verified footprint (e.g. from a SnapEDA KiCad download, or by exporting the DigiRadio EasyEDA footprint to KiCad format) with scripts/import_snapeda.py or scripts/add_component.py --name FSC-BT1035 --footprint ... -- it will detect the existing symbol and only need the footprint/model added.

Provenance

MANIFEST.csv has one row per file in the library (type, source, destination, status, hash, notes). Rows from the initial bulk import are marked UNCHANGED/baseline; rows added by import_component.py / add_component.py / import_batch.py record exactly what happened during that import (new file, deduplicated, renamed due to a real collision, or error).

Components imported from FreeDSP

The following audio/analog category chips were imported from FreeDSP_ki-CAD_Libraries (legacy KiCad .lib/.dcm format, converted to modern .kicad_sym via kicad-cli sym upgrade): ADAU1467WBCPZ300RL, PCM1808QPWRQ1, PCM9211PTR, Combo384, MW-1466CORE (FreeDSP's ADAU1466 core module), LME49720MA, CS8421-CZZ, PCM1861DBT, FDC608PZ, IMN10T108, AK5384. PCM1681-Q1 was skipped (it's a KiCad extends variant of PCM1681 and can't be split into a standalone file without duplicating PCM1681's graphics -- import PCM1681 if you need the automotive variant, base symbol is identical for schematic purposes).

Notable fixes applied during that import (see MANIFEST.csv notes for the affected files): PCM1808QPWRQ1's footprint had an absolute 3D model path pointing at the upstream maintainer's own machine (/Users/HILO/...); ADAU1467WBCPZ300RL and PCM9211PTR's footprints had two dead 3D model references each (${KICAD_USER_TEMPLATE_DIR} and a bare filename). All three were corrected to ${KIPRJMOD}-relative references pointing at the STEP files now under 3dmodels/audio/. LME49720MA was imported symbol-only, with its Footprint property repointed at this library's existing MIKILAB_ipc_soic:IPC_SOIC127P600X175-8N (an exact IPC-standard match already present) instead of duplicating a generic SOIC-8 footprint. Several FreeDSP parts already covered by the official mirrored libraries (PCM5102A, INA194, AZ1117-3.3, ADAU1452) were intentionally not re-imported.

Si4684-A10-GM (unmerged upstream MR, use with care)

symbols/audio/Si4684-A10-GM.kicad_sym (Silicon Labs/Skyworks single-chip FM/DAB/DAB+ radio receiver) was extracted from kicad-symbols MR !4782, which as of this import is open and unmerged (cannot_be_merged, has conflicts, failing CI pipeline, tagged "needs v9 format upgrade"). It is not part of the official kicad-symbols release this library otherwise mirrors. Before importing it here it was independently verified with kicad-cli sym export (parses correctly) and checked for 48 unique, non-duplicate pins matching its QFN-48 package. Symbol only -- its Footprint property points at the standard Package_DFN_QFN:QFN-48-1EP_7x7mm_P0.5mm_EP5.3x5.3mm (resolved via your global KiCad footprint table, same as other official-mirror symbols), no MIKILAB-local footprint or 3D model exists for it. Given its provenance, its pin names were cross-checked against the public Skyworks product summary -- all 24 signal names in that document's block diagram (RFREF, VHFI, VHFSW, LOUT, ROUT, DCLK, DFS, DOUT, SCLK, SSB, MISO, MOSI, VIO, VA, VCORE, VMEM, XTALI, XTALO, NVSCLK, NVSSB, NVMOSI, NVMISO, INTB, RSTB) are present with sensible pin numbers, and the remaining pins (ABYP/DACREF/DBYP bypass, SMODE, 4x GNDD, several NC) are consistent with a 48-pin QFN. That 4-page public summary does not include a full numbered pinout table, though (Skyworks gates the full Si468x datasheet behind an NDA). As a second, independent cross-check, the pin numbering was compared against the SI4684/SI4684 SMD symbols in PE5PVB/SI4684-DAB-Receiver (a built, gerber-fabricated real project) -- of the 44 pin numbers directly comparable (PE5PVB's symbol also carries an unrelated second IC's pins under duplicate numbers, and its own naming has 4 clear typos: NVCLK/DSF/MVMISO/NVMOS vs. the grammatically-consistent NVSCLK/DFS/NVMISO/NVMOSI), all 44 agree exactly with the symbol imported here. That two independent, unrelated sources converge on the same pin map is reasonably strong (if still not authoritative) confirmation; verify against the full NDA'd datasheet if you have access before finalizing a schematic around this part.

Espressif modules

19 module symbols (each with footprint + 3D model) were imported from the official espressif/kicad-libraries repository: ESP32-C3-MINI-1, ESP32-C3-WROOM-02, ESP32-C5-WROOM-1, ESP32-C5-WROOM-1U, ESP32-C6-MINI-1/U, ESP32-C6-WROOM-1, ESP32-H2-MINI-1, ESP32-MINI-1, ESP32-S2-MINI-1, ESP32-S2-SOLO, ESP32-S2-WROOM, ESP32-S2-WROVER, ESP32-S3-MINI-1, ESP32-S3-WROOM-1, ESP32-S3-WROOM-2, ESP32-S31-WROOM-3, ESP32-WROOM-E, ESP32-WROVER-E, ESP8684-WROOM-02C/U. Bare SoC/die symbols (ESP32, ESP32-C3, ESP32-S3, ESP8266, ...) and DevKit board symbols were skipped -- they have no footprint of their own (dies) or aren't components you'd place on your own board (dev boards). ESP32-S31-WROOM-3 replaces an earlier easyeda2kicad.py-exported version that had a fatal unquoted-URL syntax error in (generator ...) (see the earlier commit fixing that bug) -- the official symbol/footprint is used now instead.

All 19 footprints originally referenced their 3D model via ${KICAD8_3RD_PARTY} / ${KICAD9_3RD_PARTY} (the path KiCad's Plugin and Content Manager uses when a library is installed through it). Since this library is not PCM-installed, that variable is never defined here; the references were repointed to ${KIPRJMOD}/3dmodels/microcontrollers/ using the STEP files copied in alongside each part, so every model resolves without needing PCM or any extra KiCad configuration.

Source safety

This library was built by copying (never moving) from external source repositories; none of those repositories are modified by anything in scripts/, and nothing in this library references them. In particular, this directory does not depend on kicad-personal-library in any way — verify at any time with:

grep -R "kicad-personal-library" .

which is expected to return no matches outside of historical mentions in this README/docs.