Skip to content

yacc1-cf-card v1.0 — KiCad design (generated from cf_netlist.py)

Not built (never ordered). This design is the basis for the CF section planned on the memory card (decided 2026-09-24: same circuit, I/O-mapped on P8/P9, as the ROM and both emulators use; not designed yet). Theory: docs/cards/cf.md.

The YACC1 CompactFlash card: a CF card in a commercial CF-to-IDE adapter, driven in 8-bit True IDE mode through two I/O ports. P8 (write) is a 74LS175 latch holding the ATA register number (DA0-2) and a CF-reset bit; P9 (read/write) is the selected ATA register through a 74LS245. A 74LS138 decodes the port and a 74LS32 gates the bus strobes. Theory of operation: docs/cards/cf.md.

The circuit lives in cf_netlist.py (parts, nets, no-connects, check()). gen_cf.py draws the schematic and places the board from it; build.sh routes, checks and makes the fab files. To change the card, edit cf_netlist.py and re-run build.sh. If you hand-edit the schematic or board in KiCad instead, stop running gen_cf.py (it rewrites both) and say so here: from then on the KiCad files are the master and compare_netlist.py tells you whether they still match cf_netlist.py.

MASTER marks this folder as hand-maintained (not written by tools/eagle_to_kicad_all.py).

Files

File What it is
cf_netlist.py the circuit (single source): 26 parts, 46 nets, 23 documented no-connect pins
gen_cf.py writes the schematic, the placed board, the project and the local libraries (KiCad's Python)
build.sh the whole pipeline, below; exit status 0 = every gate passed
compare_netlist.py the netlist proof: schematic and board vs cf_netlist.py, pin for pin
yacc1-cf-card.kicad_pro project: design rules (0.25 mm min track/clearance; net class Default 0.3 mm track / 0.25 mm clearance, via 0.8/0.4; class Power = VCC, GND, PIN20: 0.6 mm track / 0.3 mm clearance, via 1.0/0.5; 0.5 mm copper-to-edge)
yacc1-cf-card.kicad_sch schematic, one A3 sheet in functional groups (bus connector, decode + strobe gating, P8 latch, data buffer, IDE header + pull-ups + adapter power, LEDs, power + decoupling, design notes); no text overlaps anything and nothing leaves the frame (tools/kicad/sch_overlaps.py: 0 / 0 / 0, frame 0)
yacc1-cf-card.kicad_pcb the routed 2-layer board
yacc1-cf-card.ses the Freerouting result imported into the board
blank-card-v3.2-eagle.kicad_sym local symbol FABC96R: the bus connector as three 32-pin units (rows a/b/c), pin numbers A1..C32, pin names = the V3.2 bus signals (from the blank card's pads); 5.08 mm pins so the three-character pin numbers clear the body and the no-connect flags
blank-card-v3.2-eagle.pretty/FABC96R.kicad_mod the bus connector footprint, copied unchanged from hardware/bus/blank-card/kicad/v3.2/
sym-lib-table, fp-lib-table the two local libraries (${KIPRJMOD}, nothing outside this folder)
yacc1-cf-card-schematic.pdf schematic plot
yacc1-cf-card-placement.pdf parts placement (silk + fab + outline)
yacc1-cf-card-render-top.png 3D render, top
yacc1-cf-card-bom.csv bill of materials from the schematic (grouped by value + footprint)
gerbers/, yacc1-cf-card-gerbers.zip F/B copper, mask, silk, Edge.Cuts, Excellon drill (mm) + drill map, job file
reports/ DRC and ERC (.rpt + .json), the schematic netlist (.net), netlist-proof.txt, Freerouting logs

Rebuild

hardware/cards/cf/kicad/v1.0/build.sh            # ~1 minute; NOROUTE=1 skips routing and fab files
  1. gen_cf.py: local libraries; the schematic (KiCad standard symbols from 74xx, Device, Connector_Generic, power, embedded in lib_symbols; every pin gets a short wire stub to a net label or a power symbol, no-connect flags on the NO_CONNECT pins and the 69 bus pins the card does not use; Reference/Value go where the library puts them unless that is on the body (the 74xx gates) or drawn rotated (R, C, LED): then above/below the body, or beside it for parts with pins only top and bottom (auto_fields()); KiCad re-saves it with kicad-cli sch upgrade); the board, started from a copy of the blank V3.2 card (outline, X1 at its place, the site text; its own power LED and 330R removed because their footprints and values differ from the netlist's LED1/R7), every footprint from PARTS, every pad on its net, GND pours on both layers, 4 mm copper keepouts round the two DIN mounting screws; each footprint linked to its symbol (DRC schematic parity is clean).
  2. Specctra DSN without the pours (tools/kicad/kicad_route.py export_dsn), so GND is routed as tracks.
  3. Freerouting 1.9 (-mt 1, 20-minute watchdog). About 30-40 s here (auto-route ~4 s, then the optimizer).
  4. Import, straight-stitch any trivial 2-pad net the router missed, pull edge-hugging tracks in, fill the pours, and give any GND pad whose thermal spokes land on a local fill island a solid pad-level connection (such a pad is already track-routed; the build log names them, typically 3-7 IC/cap GND pins; the set varies run to run).
  5. DRC with schematic parity. 6. ERC. 7. Netlist proof. 8. Gerbers, drill, zip, placement PDF, render, BOM, schematic PDF.

Freerouting is not fully deterministic: each rebuild gives a slightly different (equally valid) routing.

Results (build of 2026-09-23)

  • Netlist proof: MATCH. The netlist KiCad exports from the schematic and the pad nets of the board each equal cf_netlist.py exactly: 46 nets, 171 net pins, same names; the 92 unconnected pins are exactly the 23 NO_CONNECT pins plus the 69 unused bus pins; all 26 parts with their values and footprints (reports/netlist-proof.txt).
  • DRC: 0 errors, 0 unconnected, schematic parity 0. 8 cosmetic warnings, all inherited from the blank card's connector footprint: 4 silk_edge_clearance (X1's outline silk reaches the board edge) and 2 + 2 text_height / text_thickness (X1's 0.73 mm "1"/"32" row markers).
  • ERC: 0 errors, 1 warning: isolated_pin_label on SRST, U3 Q3 (latch bit 3, true output), which is a one-pin net by design (a probe point; the card uses -Q3 = -SRST).
  • Board 177.83 x 114.02 mm (the blank V3.2 card outline), 2 layers, through-hole only; 26 parts (5 ICs, X1, J1, J2, JP1, RN1, R1-R7, LED1-3, C1-C6); ~500 track segments, ~20 vias; signals 0.3 mm, VCC/GND/PIN20 0.6 mm, GND pour both sides.

Notes on names

  • PARTS names Device:CP for C6; KiCad 10 calls that symbol Device:C_Polarized (same pins, 1 = +), which the schematic uses.
  • Schematic label nets are named /NAME by KiCad (sheet prefix); the board uses the same names so "Update PCB from Schematic" is a no-op. compare_netlist.py strips the /.

Before ordering (for a human)

  1. Check the CF-to-IDE adapter against J1: which way the adapter plugs on (pin 1 is the square pad, top left, marked "1" on the silk; the shroud key faces the ICs), how far its body overhangs the board and whether it clears R1-R4, RN1, JP1 and the LEDs, and whether it needs the card-edge side free.
  2. Check the adapter's power input: J2 is a plain 1x4 0.1" header, pin 1 = +5 V, 2 and 3 = GND, 4 = not connected; confirm the cable/connector the adapter in hand takes (floppy Berg vs. 0.1") and the pin order. Fit JP1 only if the adapter takes +5 V on IDE pin 20 (many do not, and pin 20 is the key position on keyed cables).
  3. LED colours and the 1k series resistors (~2.5 mA) to taste.
  4. Optional hand tidying: placement is functional, not beautiful (IC row at the connector, pull-ups beside J1, LEDs bottom right); the router's track layout can be cleaned up in pcbnew. Re-run DRC and compare_netlist.py after any hand edit, and stop using gen_cf.py once you do.
  5. Check the X1 footprint's position against a real blank V3.2 card / backplane (it is copied from the blank card conversion, which was not fabricated).

Last updated 2 October 2026