Placard

KiCad project

The Placard schematic and PCB layout, one KiCad project (made in the KiCad 7 file format, so KiCad 7, 8 and 9 all open it; a newer KiCad upgrades the files when it saves them).

The board is 290 x 215 mm (290 wide, the keyboard's width; 215 deep, so kit builders have room), 4 layers, with the outline, dimensions, user connectors, cartridge slot, expansion slots, and mounting holes placed by src/scripts/gen_kicad_pcb.py (run with python3.12, which KiCad 7's Python module is built for; --png also draws docs/hardware/placard_board_layout.png). The back edge carries USB-C power, audio line out, VGA and the stacked PS/2; the left side the power switch, reset button and SD card; the right side the two SNES ports. The cartridge and the four expansion cards stand up through the case top at the back, behind the keyboard, which lies over the front 65 mm. Rerunning the script moves only the parts it places. It also places every other part as a fit test, unrouted (docs/hardware/placard_placement.png): six rows of socketed chips 35 mm apart, spread across the width, every DIP on KiCad's _Socket footprint with 2.5 mm of chip-puller room clear past each socket end, Cn 1 mm beside Un, and the script reports courtyard overlaps (KiCad DRC) and puller-room conflicts. The footprints KiCad has no part for (cartridge slot, expansion slots, PS/2, SNES, the two switches) are written by src/scripts/gen_kicad_connectors.py from typical dimensions and are preliminary: check their holes against the datasheets before ordering. Their 3D models (src/scripts/gen_kicad_3d_models.py, picture in docs/hardware/connector_3d_models.png) are drawn at typical dimensions too, with the leads put on the footprint pads. J4 (SD), J7 (VGA), F1 and SW2 use project copies of KiCad's footprints (placard: library) only so they can point at the project's models; the pads are KiCad's. The schematic rules (which chips go on which sheet, numbering, and how the sheets are drawn) are in docs/hardware/SCHEMATIC_PLAN.md. Parts and U-numbers come from docs/architecture/CHIPS.md; the PLD pinouts come from the .pld files in src/.

Every part carries Manufacturer and MPN fields (empty where no part number is chosen yet), set from the MPN table in src/scripts/gen_kicad_schematic.py, so KiCad's BOM export lists them. src/scripts/gen_bom.py writes one grouped bill of materials per assembly (main board, 64K and 32K cartridges, case), indexed in docs/bom/BOM.md, each as .md and .csv, including the bare PCBs, sockets, shells and screws that are not on the schematic.

Backups, autosaves, lock files, *.kicad_prl (per-user view settings) and fp-info-cache are git-ignored.

PLD symbols

src/scripts/gen_kicad_symbols.py writes lib/placard.kicad_sym from the PIN statements in src/pld/*.pld; rerun it after changing a PLD's pins (it overwrites the whole library). The pins are placed for the schematic, not in pin-number order: the script's LAYOUT table puts inputs on the left and outputs on the right, buses together in bit order, and each function's pins in their own group. Where one PLD does two unrelated jobs (the audio PLD's /AC_SEL, the port PLD's pad read, the memory control's RUN input) a dashed line across the box separates them. Active-low pins are /NAME, VCC (24) is on top and GND (12) underneath, unused pins are nc (no-connect type), and the .pld file name is under the part number. The script stops if a .pld's pins and its LAYOUT entry no longer match. Each symbol has the footprint Package_DIP:DIP-24_W7.62mm and the ATF22V10C datasheet link.

Other symbols

src/scripts/gen_kicad_parts.py writes lib/placard_parts.kicad_sym, in the same style, for the parts KiCad's libraries do not have: the AS7C256C SRAM, the expansion slot (Molex 87715-9106 as the cartridge slot, contacts A1-A32 and B1-B32) and the cartridge slot (Molex 87715-9106, 2 x 32 keyed, contacts A1-A32 and B1-B32), as in EXPANSION.md, with the +5 V and GND contacts stacked on one pin each, the SNES pad socket (IO.md) and USB_C_Power, the 5 V input: a power-only 6-contact USB-C receptacle (GCT USB4125, footprint placard:USB_C_Receptacle_GCT_USB4125_6P_HandSolder: KiCad's USB4125 footprint with the SMD pads 1.5 mm longer for the iron, made by gen_kicad_connectors.py) with a 5.1k resistor from CC1 and from CC2 to GND so a charger gives 5 V. Make changes in the script, since rerunning it overwrites the library.

Every symbol, footprint and 3D model the sheets and boards use is in lib/ (since 2026-10-26): the projects' library tables list only the placard libraries, so the project opens the same on any PC and DRC/ERC find nothing missing or different from its library. The parts below started as KiCad library parts and are used through their copies in placard_std and placard.pretty:

Set the Value to the real part number when placing them. src/scripts/render_kicad_symbols.py OUTDIR draws all of these as PNG review sheets (needs kicad-cli, cairosvg and Pillow).

Schematic sheets

src/scripts/gen_kicad_schematic.py writes all the .kicad_sch files (main board and cartridge) from its pin-by-pin net lists, so change a connection there and rerun it; a hand edit in KiCad is lost at the next run. Nets with two or more pins on a sheet are wired by the small router in src/scripts/kicad_route.py, and numbered groups (D0-D7, ...) are drawn as one bus per sheet (docs/hardware/SCHEMATIC_PLAN.md, "How the sheets are drawn"). --check compares KiCad's exported netlist with the script's nets and runs basic electrical checks; the full ERC needs KiCad 8 or newer (open the project, Inspect > Electrical Rules Checker). PDFs of both are in ../schematics/.

Dimension drawing

../docs/hardware/placard_main_dimensions.pdf is a three-sheet mm drawing of the main board: outline and mounting holes, edge connector positions, and the expansion card and cartridge space. It is made by src/scripts/gen_board_dimensions.py, which needs KiCad 9 (pcbnew Python and kicad-cli). The script never writes placard.kicad_pcb: it adds KiCad dimension objects on Dwgs.User in temporary copies and plots those, so rerun it after the layout changes.