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
gen_cf.py: local libraries; the schematic (KiCad standard symbols from74xx,Device,Connector_Generic,power, embedded inlib_symbols; every pin gets a short wire stub to a net label or a power symbol, no-connect flags on theNO_CONNECTpins 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 withkicad-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 fromPARTS, 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).- Specctra DSN without the pours (
tools/kicad/kicad_route.py export_dsn), so GND is routed as tracks. - Freerouting 1.9 (
-mt 1, 20-minute watchdog). About 30-40 s here (auto-route ~4 s, then the optimizer). - 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).
- 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.pyexactly: 46 nets, 171 net pins, same names; the 92 unconnected pins are exactly the 23NO_CONNECTpins 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 + 2text_height/text_thickness(X1's 0.73 mm "1"/"32" row markers). - ERC: 0 errors, 1 warning:
isolated_pin_labelonSRST, 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¶
PARTSnamesDevice:CPfor C6; KiCad 10 calls that symbolDevice:C_Polarized(same pins, 1 = +), which the schematic uses.- Schematic label nets are named
/NAMEby KiCad (sheet prefix); the board uses the same names so "Update PCB from Schematic" is a no-op.compare_netlist.pystrips the/.
Before ordering (for a human)¶
- 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.
- 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).
- LED colours and the 1k series resistors (~2.5 mA) to taste.
- 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.pyafter any hand edit, and stop usinggen_cf.pyonce you do. - 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