Skip to content

memory-v2.0 — the built memory card v1.3 + the CompactFlash interface (KiCad design)

ORDERED from JLCPCB 2026-10-09, order 2000765A-Y52 (Ken; shown by JLCPCB as Y52-2000765A; memory-v2.0-gerbers.zip, 4 layers, the settings in memory-v2.0-jlcpcb-order.txt; not yet received or built). The zip was re-verified against the board that day: every layer and both drill files match. Ordered with three items still open, by Ken's choice: the BASIC RUN fault on the machine (BACKLOG.md; v2.0 shares v1.3's ROM -CE/-OE path), the unexplained jumper wire on the built card's IC7 pin 4, and the ribbon plug's pin 20 (a cable choice).

Status 2026-09-30: THE v2.0 BOARD IS STANDOFF OPTION E (chosen 2026-09-25), FINISHED FOR FABRICATION; 2026-09-29: + JP3, the ROM write-protect jumper; 2026-09-30: + R15, the ADDR15 pull-down ("The ROM write-protect jumper JP3" and "The ADDR15 pull-down R15" below). memory-v2.0.kicad_pcb (beside the schematic, sharing memory-v2.0.kicad_pro / .kicad_dru): the CF-to-IDE adapter (an HX-2118P, measured) flat on two 15 mm M3 standoffs over the CF chips at the free top edge, fed by a short straight 40-wire ribbon from J2, the card's own IDE header, parallel to the bus connector X1; the ROM uncovered in the top row of the memory column. Routed (0 unrouted, 72 through vias, 12,808 mm), DRC 0 copper violations and 0 unconnected, planes one piece each, netlist proof MATCH, silkscreen tidied, fab files made: see "The v2.0 board" below. Open before ordering: only the ribbon plug's pin 20 (the adapter's power-pad order was resolved 2026-09-26: floppy pinout, a straight-through cable from J3, a hand-made harness). The 1:1 print changed with JP3 and again with R15: reprint memory-v2.0-1to1.pdf before ordering.

The records: the five standoff placement options A-E with their trial routes and 1:1 check prints ("The standoff options", "The standoff options C / D / E"), and the board finished earlier on 2026-09-24 from top-edge option B (J2 at the free top edge, the TAODAN adapter standing on it; routed, 43 vias, fab files), kept as a record in options-top-edge-J2/ with the three top-edge re-layout options and their trial routes ("The top-edge record").

v2.0 is the memory card v1.3 as built (../v1.3: the KiCad conversion of the Fusion 360 export (2026-09-24) of the card JLCPCB fabricated on 2025-06-27, proven against the order's gerbers; 62256 x 2, 28C64, IC7 block decode, FORCE-ROM, IC15 buffer enable, TMP0/TMP1) minus C20-C23 (four spare 100 nF, below) plus the CompactFlash interface of the CF card v1.0 (../../../cf/kicad/v1.0/), as drawn: its own 74LS138 decoding I/O ports P8 (register-select latch, write) and P9 (data, read/write), enabled by IO-ADDR3. The ROM in the machine and both emulators (software/cfmodel.h, firmware/monitor/monitor.asm) already talk to P8/P9: no firmware change. The CF card's own bus connector goes; the CF section shares the memory card's X1. Theory of the CF circuit: docs/cards/cf.md; of the memory card: docs/cards/memory.md.

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

History: the first v2.0 (0c2e15e) was drawn on what was then ../v1.3 (now ../deprecated/v1.3-do-not-use), an earlier save of the design without IC15 and without the TMP registers' copper. Rebuilt on the real design (the Fusion 360 export, 4365de6), the CF section no longer fitted beside the built card's copper (its DATA8-15 bundle crosses the free area): options A/B/C with the built copper kept were all blocked. Decided 2026-09-24: re-lay the whole card (way 4 of that list). The blocked options are kept as a record in options-keep-copper/ (below).

Rename, 2026-09-24: the built card's folders eagle/v1.3-fusion-export-2026-09-24 and kicad/v1.3-fusion-export-2026-09-24 became eagle/v1.3 and kicad/v1.3; the earlier save moved to eagle/deprecated/v1.3-do-not-use (KiCad kicad/deprecated/v1.3-do-not-use). The conversion was regenerated under its new project name memory-v1.3, so its library nickname is now memory-v1.3-eagle and, because the converter derives schematic UUIDs from the project name, its symbol and sheet UUIDs changed. Here that meant: BASE_NAME / BASE = v1.3, the copied libraries renamed memory-v1.3-eagle.* (lib tables and every lib_id follow, regenerated by gen_mem_v2.py sch), and in the committed boards that are not regenerated by a NOROUTE=1 build (the three trial routes and the three keep-copper records) the 53 v1.3 footprints' library ids and schematic paths were rewritten to the new names/UUIDs (matched by reference designator; the 21 CF footprints' paths did not change). Nothing else in those boards changed: every track, via, arc and zone is byte-identical, and NOROUTE=1 build.sh passes with the same numbers as before (0 unrouted, 43 vias, no copper violation, no new parity item, netlist proof MATCH for all nine boards).

The v2.0 board: standoff option E, finished for fabrication (chosen 2026-09-25)

memory-v2.0.kicad_pcb, made by finish_v2.py make-e from a route of options-standoff/memory-v2.0-standoff-e.kicad_pcb (the placement of option E, unchanged: "The standoff options C / D / E" below). ORDERED 2026-10-09 (JLCPCB).

The placement (option E). X1 | column 1 (the TMP registers IC27 / IC29 / IC26 / IC28, the address buffers IC9 / IC8, RN5 / RN6) | column 2 (glue, IC5) | column 3 = the memory column: the ROM IC13 in the top row (uncovered, removable: its keep-clear zone of 10 mm past both short ends and 2 mm along the sides holds nothing and is 5.1 mm from the adapter), then IC1, IC2, IC15 | J2 (2x20 shrouded, rotation 180: pin 1 = the square pad at the y-max end, odd row x 144.75, pin 1 at (144.75, 110.03)) | the HX-2118P adapter x 151.04-195.04, y 55.90-115.90 (its CF slot edge 0.49 mm inside the top edge), 3.0 mm from J2's shroud (J2's 18 mm plug envelope 1.5 mm clear of it), on standoffs H1 (166.34, 111.90) and H2 (166.34, 59.90), 52.0 mm apart: MountingHole_3.2mm_M3, 3.2 mm NPTH, each in a 7 mm keep-out on all four copper layers (no track, no via, no plane). Under the adapter only sockets, disc caps and axial resistors: IC32 / IC31 / IC34 (+ C27 / C26 / C29) in its header half, IC33 (+ C28) beside H1, R10-R13 and RN9. J3 (adapter power) just outside the adapter's y-min edge beside its power pads, C30 beside it; IC7 / IC4 / IC30 in the JP1 top-edge corner beside the U$1 jumpers; the LEDs PWR0 / LED1 in the y = 124 top-edge corner; JP2 past J2's pin-1 end, OPEN by default (the HX-2118P has no pin 20). gen_standoff.py check passes on the finished board (reports/memory-v2.0-placement-check.txt). No part was moved after routing (finish_v2.E_NUDGE is empty); the only changes are silkscreen texts (below).

The ROM write-protect jumper JP3 (2026-09-29; mem_v2_netlist.py rule 7)

Why. On v1.3 the 28C64's -WE (IC13 pin 27) is -MEM-WR re-buffered by IC6, the same net as the RAMs' -WE, with nothing to stop a write: any store while the ROM is selected writes the EEPROM - and during FORCE-ROM every address selects it (design review M2, hardware/cards/memory/reviews/v1.3-datapath-2026-09-21.md; docs/cards/memory.md section 4). The chip then spends ~10 ms in its internal write cycle, returning poll bits instead of code, and the byte stays changed. The monitor avoids it only by jumping above $8000 first; the reset-time window (finding 1.3: a stale control word with -MEM-WR asserted while reset is held) it cannot avoid.

What. IC13 pin 27 leaves the -WE net for its own net, ROM-WE, and JP3 picks what drives it:

JP3 IC13 -WE use
2-3 PROTECT (fit it here) held at VCC: the EEPROM can only be read always, in the machine
1-2 WRITE -MEM-WR, exactly as v1.3 only to write the 28C64 in place (nothing does today: it is burned in a programmer)
no cap floating: do not run without one

JP3 is v1.3 JP1's part (3-pin header, footprint 1X03, BOM line "JP1,JP3"). On the schematic (sheet 3, gen_mem_v2.add_wp_jumper()) the -WE wire to pin 27 now runs to JP3 pin 1, a ROM-WE label joins pin 27 to JP3 pin 2, pin 3 goes to VCC, and a note says how to set it. On the board it is a local change (finish_v2.add_wp(), run by make-e and by finish_v2.py wp): JP3 sits in the free patch above-left of the ROM at (96.04, 27.30) (pad 2; outside the ROM keep-clear zone, which starts at y 31.9), silk "JP3 ROM WE / 1-2 WRITE / 2-3 PROT" above it and a "1" under pin 1 (RN8's own "1" sits just right of JP3's pin 3). Copper: the -WE run from IC6 no longer meets at IC13 pin 27 - its F.Cu track ends in a new via at (104.44, 38.60) onto the same B.Cu run to IC1 / IC2 pin 27; JP3 pad 1 joins that F.Cu run through a via at (93.50, 37.60); ROM-WE leaves pin 27 on F.Cu under the pin row (y 36.8) to a via at (96.04, 36.80) and B.Cu up to JP3 pad 2; pad 3 is on the VCC plane (In2.Cu), no track. Four -WE tracks replaced, 10 added, 3 vias more; every other track of the route is unchanged. add_wp() is drawn for this board's route (FINAL=route SEEDS=15) and stops with an error on any other (for instance FINAL=trial, whose route differs): there JP3 would have to be placed anew. Boards made before rule 7 (the standoff options, their trial routes, the records) keep IC13 pin 27 on -WE; the netlist proof and the DRC parity gate check them against the schematic without JP3 and require JP3 on this board.

The ADDR15 pull-down R15 (2026-09-30; mem_v2_netlist.py rule 8)

Why. The fix for design review M1, the FORCE-ROM race: between bus cycles nothing drives ADDR15 and an undriven LS input reads high, so IC12's clock (ADDR15 · VMA · BUS-EN) can clear FORCE-ROM before the real address arrives; 470 Ω to GND holds the line low until a driver puts a 1 on it. The why, the value and the loads: docs/cards/memory.md section 4.1.

What. R15, 470 Ω, 1/4 W, from ADDR15 (pin 1) to GND (pin 2). The same part as the CF section's R10-R14 (Device:R, footprint Resistor_THT:R_Axial_DIN0207_L6.3mm_D2.5mm_P10.16mm_Horizontal), and the next free reference (the built card has R2, the CF section R10-R14). pd_apply() checks that the net ADDR15 is exactly IC10 pin 4 (the FORCE-ROM clock gate), IC9 pin 17 (the address buffer) and X1 pin A18 (the bus) before it adds R15. On the schematic (sheet 2, the FORCE-ROM logic; gen_mem_v2.add_pulldown()) R15 hangs from the ADDR15 wire into IC10B pin 4 through a junction, with a GND symbol and a note ("R15 470: ADDR15 pull-down, FORCE-ROM race fix ...").

On the board (finish_v2.add_pd(), run by make-e after add_wp() and by finish_v2.py pd): a local change, like JP3. Nothing near IC10 or IC9 has room for a 12 x 3 mm resistor without moving parts, so a search of the committed route for a spot where R15's courtyard meets no other part and both pads keep 0.2 mm from every other net found one: the strip between the bus connector X1 and the cap column C16 / C4, R15 lying parallel to X1 with pad 1 at (32.58, 65.56) right on the ADDR15 track (its 45-degree F.Cu run from X1 A18 towards IC9) and pad 2 at (32.58, 75.72) on GND, which reaches the In1.Cu plane through its thermal relief like the card's other GND pads. Copper: the one ADDR15 track under pad 1 is split at the pad centre into two; nothing else is added (no track, no via), every other track of the route is unchanged. Clearance from pad 1 / pad 2 to the nearest other net: 0.36 / 0.33 mm (ADDR14 / ADDR11, F.Cu). Silk: "R15" and "470" inside its body outline (0.8 mm, reading upward); C16's reference moves from the left of C16 (now under R15's pad 1) to its right, between C16 and IC28. add_pd() is drawn for this route and stops with an error on any other, as add_wp() does. Boards made before rule 8 (every board but this one) have no R15: the netlist proof and the DRC parity gate check them against the schematic without it and require R15 on this board.

Which route. Two candidates, compared by build.sh's rule (fewest unrouted, then vias, then length):

route unrouted vias track
E's committed trial route (options-standoff/memory-v2.0-standoff-e-trial.kicad_pcb, best of DSN component orders 0-7) 0 72 12,579 mm
20 new Freerouting runs, component orders 8-27 (same settings: 30 passes, -oit 100, one thread) 0 in 10 of 20 (69-92 vias) 69 (order 15) 12,668-12,856 mm (complete runs)

Order 15 is kept: 69 vias, 12,783 mm (3 vias fewer, 204 mm = 1.6 % more track). The new runs shared the machine (20 runs in two waves of 10), which is why so many stopped with one connection left; the kept one is complete. The board was then made with FINAL=route SEEDS=15 build.sh, which routed that order again and got the same route (69 vias, 12,783 mm: Freerouting repeats itself for one file; reports/memory-v2.0-order.txt, -freerouting.log).

Clean-up (finish_v2.py make-e, the same passes as on the top-edge board): - Vias: all 69 are through vias (0.8 / 0.4 mm): gen_relayout.py ses converts the session import's "buried" vias on import, make-e converts any left and verify checks it. - Needless vias: each via's one-layer runs were tried on the other signal layer (keeping clearance, edge distance and T-junctions): none could go (66 of the 69 blocked by another net's track there; the rest by runs that end in a branch, a T-junction or another net's pad). 69 vias stay (72 since JP3, 2026-09-29). - Collinear segments merged: 2,049 -> 2,038 segments, no geometry change. - The standoff keep-outs hold no copper (the DRC's rule-area check: 0 items).

Silkscreen (finish_v2.py make-e; checked by finish_v2.py verify and the DRC: no text on a pad, via, hole, other silk or the edge, none upside down; DRC silk_overlap 0): - "YACC1 MEMORY BOARD V2.0" (the built card's title, same place), "onepagecomputer.com" kept. - The adapter outline (60 x 44 mm, 0.15 mm lines) where the adapter sits, cut around pads, vias and other silk; its slot side drawn 0.2 mm inboard of the slot edge (that edge is 0.49 mm from the board edge; silk keeps 0.5 mm). Inside it: "CF ADAPTER ON 15 mm STANDOFFS", "ADAPTER PIN 1" at its pin-1 end (beside J2's pin 1), "CF CARD INSERTS HERE" along the slot edge, a circle where each standoff stands with "H1" / "H2" beside it. - J2: "IDE" beside the shroud, "PIN 1" at the square pad (J2's pin-1 triangle from the library), "CF: P8/P9" past its pin-1 end. - "ROM - removable" under IC13's reference, in the ROM's body outline. - J3: one label per pin above it, +5V, G, G, nc (pin 1 = +5V, square pad). - JP2: "PIN20 +5V (open for HX-2118P)" beside it. - LEDs: "ACT" left of LED1, "PWR" between LED1 and PWR0 (next to PWR0). PWR0's own reference had no free spot on the silk (IC33 above, the board edge below, the "PWR" label beside it, too small inside its outline): it is on F.Fab (the placement PDF), the one reference not on the silkscreen. - The block-removal jumper labels ROM / RAM / 0X8000 / 0XF000 at U$1, the "1" marks of RN7 / RN8, "-BUS-EN" and "Gnd" at JP1 (as on the top-edge board: "Gnd" beside pin 3). - Every IC's reference in the middle of its body (its value on F.Fab), every other reference beside its part; 51 texts moved by the tidy (most 0.3-0.5 mm; LED1 5.1 mm, J2 3.3 mm, JP2 2.7 mm; of the new labels "IDE" 6.6 mm, into the shroud's key notch, "ADAPTER PIN 1" 3.0 mm, "PIN 1" 2.8 mm), R2's turned upright. - F.Fab keeps the full adapter drawing of the option board (outline, holes + standoff circles, its header shroud and pin-1 end, power pads approx., CF slot edge, J2's plug envelope, the ribbon arrows, the ROM keep-clear zone and the texts): it is on the placement PDF, not on the gerbers. The option board's User.Drawings copy and captions are gone.

Final numbers (reports/memory-v2.0-final.txt, -drc.json, -drc.rpt)

v2.0 board (standoff E) the top-edge record the built card v1.3 (its own rules)
unrouted 0 0 0
vias 72, all through, 0.8 / 0.4 mm (69 + JP3's 3; R15 adds none) 43 (0.4572 / 0.254 mm)
track 2,045 segments, 12,808 mm (F.Cu 6,853 / B.Cu 5,955; R15 splits one ADDR15 segment), all 0.25 mm; placement airwire 11,130 mm 11,779 mm 0.1524 mm tracks
DRC copper violations 0 (clearance, shorts, width, via, hole, edge, starved thermal, dangling, unconnected, rule areas) 0 0
DRC unconnected 0 0 0
planes GND on In1.Cu and VCC on In2.Cu each one piece, ~16,380 mm2 (81 % of the board after antipads and the two 7 mm keep-outs); all 176 GND/VCC pads on their plane through thermal reliefs same same stack-up
DRC items left, all inherited X1's two mounting holes in X1's own keepout 2/2, X1 library mismatch 1/1, X1 silk over the edge 4/4, X1 pin-number text height 2/2, Eagle-footprint silk outlines over pads (silk_over_copper) 199/199 same
DRC silk_overlap / text_thickness 0 / 0 0 / 0 45 / 1
schematic parity 49 items, all the built card's inherited Eagle values/fields; new: none same 220
ERC 99, PASS (the built card's 104 residue - 6 bus labels now global + the designed-in SRST label) same 104
netlist proof MATCH (72 parts + the two board-only standoff holes H1 / H2, 187 nets, 692 pads) MATCH (before JP3 and R15)
drill 4 layers; PTH file 807 holes, 6 sizes; NPTH file: H1 / H2 (3.2 mm) + X1's two 2.79 mm mounting holes (finish_v2.py drill-check) one drill file

Fab outputs (finish_v2.py fab-e; a plain build.sh run regenerates them from the committed board)

File What
memory-v2.0-gerbers.zip the upload: the 14 files of gerbers/
gerbers/memory-v2.0-F_Cu.gbr, -In1_Cu.gbr, -In2_Cu.gbr, -B_Cu.gbr copper L1 (signals) / L2 (GND plane) / L3 (VCC plane) / L4 (signals)
gerbers/memory-v2.0-F_Mask.gbr, -B_Mask.gbr, -F_Silkscreen.gbr, -B_Silkscreen.gbr, -Edge_Cuts.gbr masks, silkscreens (the bottom one is empty), outline
gerbers/memory-v2.0-PTH.drl, -NPTH.drl, -PTH-drl_map.gbr, -NPTH-drl_map.gbr, -job.gbrjob Excellon drill, plated and non-plated in separate files (mm; the NPTH file holds the standoff holes H1 / H2 and X1's two mounting holes), drill maps, Gerber job file (4 layers, 1.6 mm)
memory-v2.0-jlcpcb-order.txt the order parameters, as the built card's JLCPCB order 2000765A-Y42 (../../eagle/v1.3/fab/jlcpcb-order-2000765A-Y42.zip, YG/4te.json): FR-4, 4 layers, 1.6 mm, outer copper 1 oz, inner 0.5 oz, green mask, white silk, HASL with lead, vias plugged
memory-v2.0-render-top.png, memory-v2.0-render-bottom.png 3D renders (the adapter is shown by its silkscreen outline)
memory-v2.0-placement.pdf assembly drawing: silkscreen + F.Fab (values, the adapter drawing, PWR0) + outline, title block
memory-v2.0-1to1.pdf the 1:1 US-Letter print of the routed board (print_1to1.py: tracks F.Cu light red / B.Cu light blue, vias, parts, the adapter, holes, J2, ribbon, ROM zone; page 2 the side view and notes): print at 100 % and lay the adapter on it
memory-v2.0-schematic.pdf, memory-v2.0-bom.csv schematic (7 sheets); BOM: 36 part lines, 72 parts, then H1,H2 (3.2 mm NPTH mounting holes: board features, no part, Qty 0) and the hardware lines HW1-HW6 (below)
reports/memory-v2.0-*.txt/json/rpt -make.txt (the make-e log), -order.txt (the route kept), -freerouting.log (FINAL=route only), -placement-check.txt, -drc.json / -drc.rpt, -final.txt, -fab.txt

Assembly notes

  • Hardware (BOM HW1-HW6): 2 x M3 hex standoff 15 mm, female-female (5.5 mm across flats); 4 x M3 x 6 mm screws (two through the adapter into the standoffs, two from under the card); 4 x M3 washers (7 mm OD: the holes' 7 mm copper keep-out is sized for them, no pad within 4 mm of a hole centre); one 40-wire IDE ribbon, ~5-8 cm between two 40-way IDC plugs crimped alike (pin 1 to pin 1, stripe at the pin-1 end = the y-max end of J2 and of the adapter; ~4 cm is the minimum, standoff_placements.ribbon_length()); the adapter power cable from J3; the HX-2118P itself.
  • Order: sockets and parts first (everything under the adapter is socketed DIPs, disc caps, axial resistors), then the standoffs (screws from under the card, washer under each head), the ribbon into J2, the adapter onto the standoffs (screws + washers from above), the ribbon into the adapter's header, the J3 cable to its power pads.
  • JP3: fit its jumper cap on 2-3 (PROTECT); 1-2 only to write the 28C64 in place. Never run with no cap (the ROM's -WE would float).
  • R15 (470 Ω, 1/4 W, yellow-violet-brown): an ordinary axial resistor lying flat between X1 and C16 / C4, either way round. Before using the bus tester with this card, read the tester's RN4 value (its address-line pull-ups): with 10 kΩ the idle A15 sits at ~0.2 V, fine; with 1 kΩ it would be ~1.6 V (docs/cards/memory.md 4.1).
  • Pin 20: the adapter has no pin 20 (key). J2 has it fitted. Use a ribbon whose J2-end plug has pin 20 open (generic 40-way IDC sockets are) - a keyed IDE plug (pin 20 blocked) does not go onto J2 unless J2's pin 20 is pulled. JP2 stays OPEN (pin 20 = +5 V serves adapters powered through the header, not this one).
  • Adapter power: J3 = +5V, G, G, nc (pin 1 square, labelled on the silk) to the adapter's four power pads (between its header and the H2 hole). Confirmed 2026-09-26: these adapters take a 4-pin floppy (Berg / mini-power) connector: pin 1 +5V (red), 2 GND, 3 GND, 4 +12V (yellow) - the same order as J3, so the cable is straight through, pin 1 to pin 1 (J3 pin 4 is n.c., so the adapter never gets +12 V; a CF card needs none). Before making it, identify the adapter's pin-1 pad (square pad / "1" / "+5V" silk, or meter: +5V beeps to the middle pin of its 3.3/5 V jumper, GND to IDE pin 2). Either solder a 2.54 mm 1x4 header on the pads and use a 4-wire female-female jumper to J3, or fit a Berg (2.5 mm) floppy socket and a floppy-to-2.54 lead.
  • Heights (15 mm standoffs): J2 + plug ~18 mm, CF card top ~22 mm, the adapter's plug ~35 mm, the ribbon loop ~42 mm above the card; screw heads + washers ~3 mm below. The card cage: resolved (2026-09-25) - nothing will be in front of the memory card, the slot on its component side stays empty.
  • The ROM IC13 stays reachable: nothing above it, 10 mm free past both short ends (lever it out, or a 28-pin ZIF socket later).

Open items before ordering

  1. ~~The adapter's power-pad order~~ - resolved 2026-09-26: the power harness from the CF-IDE adapter to J3 is made by hand (J3 is fixed: +5V, G, G, nc); the board does not depend on it.
  2. The ribbon plug's pin 20: pin 20 open on the J2 plug, or pull J2's pin 20 (either works; decide with the cable in hand).

Resolved: ~~the card-cage slot pitch vs the ~35 mm stack height~~ - nothing in front of the memory card (2026-09-25). Confirmed earlier: the adapter's pin 1 (straight ribbon, pin 1 to pin 1).

ORDERED 2026-10-09 (JLCPCB).

What v2.0 is, relative to the built card

  • Schematic. Sheets 1-6 are the built card's, copied unchanged except: on sheet 1 the six X1-only local labels IO-ADDR0-3, -IO-RD, -IO-WR became global labels (sheet 7 uses them) and a note says so; C20-C23 are taken out of sheet 1's cap row (the symbols go; the GND and VCC rails through their pins become one wire each from C19 to C24, their four + four junctions go; gen_mem_v2.py remove_parts()); sheet 3 gets JP3 (IC13 pin 27 onto ROM-WE, above); sheet 2 gets R15 (ADDR15 to GND, above); title blocks say v2.0. Sheet 7 is the CF section, nets shared with sheets 1-6 as boxed global labels; since 2026-10-24 drawn with its own nets as wires ("Sheet 7, the CF section, wired" below). IC15 (74ALS11, gate A = AND(-LO-RAM, -HI-RAM, -ROM-CS) -> IC5 pin 19, the 74LS245's enable) is part of the built card's schematic. The circuit is unchanged by the re-layout.
  • Bus pins now used (same backplane pinout as the CF card v1.0; checked pin by pin against the built card's X1 by check_netlist.py): IO-ADDR0-3 = C7-C10, -IO-RD = B25, -IO-WR = B26 (unused on v1.3, now wired to the CF section); -RESET = C30 (v1.3: IC12 PRE, now also IC32 CLR and IC33); DATA0-7 = A19-A26 (also IC34 A side, IC32 D1-D4).

Sheet 7, the CF section, wired (redrawn 2026-10-24)

Sheet 7 is drawn by tools/kicad/sch_wire.py (shared with the video card V2.0; ELK places the parts, the P8X project's way) on the CF card's sheet writer gen_cf.py: the decode IC30, the strobes IC31/A-C, the latch IC32, the gates IC33/A-C, the buffer IC34, the header J2 with RN9, R10-R13 and JP2, and the ACT LED (R14, LED1) are placed left to right and every net of the section with two or more pins on the sheet is a wire carrying its name once (a local label, so KiCad names it /Sheet 7/<name> as before). The bus nets shared with sheets 1-6 (DATA0-7, IO-ADDR0-3, -IO-RD, -IO-WR, -RESET) keep a boxed global label at each pin, power keeps its symbols, SRST its one-pin label. Below the drawing: J3 and C30 (the adapter's power), the unused gates IC31/D and IC33/D, the two power units and C25-C29, and the design notes. A2 (A3 before). Until 2026-10-23 every pin was a stub to a label or a power symbol in functional boxes.

Before After
nets drawn as wires 0 26 (120 wire segments, 13 junctions)
stubs (a pin to a label or power symbol) 136 70
labels 66 local, 21 global 27 local, 21 global
power symbols, no-connect flags 48, 23 48, 23

The proofs (2026-10-24; sheets 1-6 byte-identical, mem_v2_netlist.py unchanged): the netlist proof (check_netlist.py, as build.sh step 6) MATCH, reports/netlist-proof.txt identical line for line (187 nets; every board and record board = the schematic); the ERC gate (reports/erc-summary.txt) identical: 99 findings, the same as before, 1 error (sheet 3's inherited missing_power_pin), nothing new but the designed-in SRST label -> PASS; DRC of the v2.0 board with schematic parity: 0 unconnected, the same 49 parity items (the built card's inherited Eagle values and fields) as before. The board file differs only in two footprint links: IC31 and IC33, whose units now lie in another order on the sheet, carry the UUID of the unit KiCad now names first (gen_mem_v2.py link <netlist> memory-v2.0.kicad_pcb: the (path ...) lines, as "Update PCB from Schematic" would set them; nothing else). The Gerbers and drill files re-exported from it (the finish_v2.py fab-e commands, into a scratch folder) equal gerbers/ - the files of order 2000765A-Y52 - apart from their date / time lines. gen_mem_v2.py sch needs node and elkjs (cd tools/kicad && npm install).

Port assignment

Port Dir What
P8 write IC32 74LS175 latch: bits 0-2 = ATA register (CF DA0-2), bit 3 = CF reset (1 = held), 4-7 ignored
P9 read/write the ATA register P8 selected, 8-bit True IDE, through IC34 74LS245

IC30 (74LS138) takes IO-ADDR0-2, G1 = IO-ADDR3, G2A/G2B low: Y0 = P8, Y1 = P9, Y2-Y7 unused. The I/O card must keep its IO-ADDR-HL strap at P0-P7 (it would otherwise also answer P8/P9).

Part-list delta (built v1.3 -> v2.0)

Removed (2026-09-24, the unused capacitors on the memory card): C20, C21, C22, C23, the built card's four 100 nF (C-US, C025-025X050) with no IC beside them: on v1.3 they sit in the cap row between C19 and C24, pin 1 on GND, pin 2 on VCC, nothing else. v2.0 had kept them only as spare plane-to-plane decoupling (C20/C21 at X1's two power groups, C22/C23 at the far end of the planes). Every IC keeps its own 100 nF (C1-C19 and C24 for the built card's 20 ICs, C25-C29 for the CF chips) and C30 (10 uF bulk at J3) stays. mem_v2_netlist.REMOVED is the single source; the netlist proof checks that each was a plain VCC-GND cap on v1.3 and is gone from v2.0.

Added (reference designators clear of the built card's IC1-IC15, IC18, IC26-IC29, C1-C24, R2, RN5-RN8, JP1, PWR0, U$1, X1):

v2.0 CF card v1.0 Part Footprint
IC30 U1 74LS138 port decode DIP-16
IC31 U2 74LS32 strobe gating DIP-14
IC32 U3 74LS175 P8 latch DIP-16
IC33 U4 74LS08 buffer enable / CF reset / ACT driver DIP-14
IC34 U5 74LS245 P9 data buffer DIP-20
J2 J1 40-pin IDE header, 2x20 2.54 mm, shrouded (pin 20 kept) IDC-Header_2x20_P2.54mm_Vertical
J3 J2 adapter power 1x4 (1 +5 V, 2/3 GND, 4 n/c) PinHeader_1x04
JP2 JP1 IDE pin 20 = +5 V jumper PinHeader_1x02
RN9 RN1 10k x8 SIP, CF D0-7 pull-ups R_Array_SIP9
R10-R13 R1-R4 10k: IORDY, -PDIAG, -DASP pull-ups, -DMACK high axial 10.16 mm
R14, LED1 R5, LED2 1k + yellow ACT LED (any P9 access) axial, LED 5 mm
C25-C29 C1-C5 100 nF, one per new IC disc 5 mm
C30 C6 10 uF bulk beside J3 radial D5

Added on the built card's side (rule 7, 2026-09-29): JP3, ROM write-protect jumper, 3-pin header (PINHD-1X3, memory-v1.3-eagle:1X03, the same part as JP1). (Rule 8, 2026-09-30): R15, 470 Ω ADDR15 pull-down (Device:R, R_Axial_DIN0207_L6.3mm_D2.5mm_P10.16mm_Horizontal, the same part as R10-R14).

Dropped from the CF card: X1 (bus connector, shared), LED3 + R6 (DASP LED, not wanted), LED1 + R7 (PWR LED: the memory card already has PWR0 + R2 330R). Everything through-hole. BOM: memory-v2.0-bom.csv (36 lines, 72 parts: the built card's 53 - C20-C23 + the CF section's 21 + JP3 + R15; built-card parts keep their converted Eagle values, e.g. 74*32, C-US, whose line is now C1-C19,C24 x 20).

The standoff options (2026-09-24: the CF adapter on standoffs on the card)

The decision

  • The CF-to-IDE adapter is an HX-2118P and mounts flat on two M3 standoffs on the memory card, component side up, its header edge toward the bus connector and its CF slot toward the free top edge (a CF card is pushed in toward the bus).
  • J2 runs parallel to X1 (long axis along y) about 1/3 of the way from the bus edge to the top edge, just beside the adapter's header edge on the bus side, not under the adapter; a short straight 40-way ribbon (two IDC plugs) arches from J2 up to the adapter's header.
  • The ROM (IC13, 28C64) must stay removable (it is pulled and reburned): nothing above it (adapter, standoffs, ribbon) and room around it to lever it out or fit a ZIF socket later.
  • The LEDs stay where they were (PWR0 / LED1 in the free top-edge corner at y = 124); X1, the outline, X1's mounting holes, JP1 and the U$1 block jumpers (RN7 / U$1 / RN8, with IC18 / C24 beside them) as before; the circuit is the same (netlist proof MATCH), the 4-layer stack-up and the re-layout rules are the same.

The adapter (measured from a photo, confirmed with a 1:1 print)

"View" = component side up, IDE header at the top.

board 60.0 mm (along the header) x 44.0 mm
IDE header male 2x20, 2.54 mm, shrouded, along one 60 mm edge; pin 20 missing (the key: the adapter cannot take +5 V through IDE pin 20); pin rows ~4.6 / 7.1 mm from the edge (template)
pin 1 at the left end of the header (measured "left end of the outer row", see open question 1)
holes two only, both at the header end: 52.0 mm apart (+/- 0.7), centred on the header, 15.3 mm from the header edge, ~4 mm in from the side edges, ~3.2-3.5 mm (M3)
CF slot opens at the far edge, 44 mm from the header edge
power four unpopulated pads in a row between the header and the holes, just inboard of the right-hand hole (view); probably +5V / GND / GND / +12V, floppy style (to confirm). No power through the IDE connector (no pin 20): J3 (+5V, G, G, nc) feeds the pads by a short cable

On the board (the adapter turned so its header edge faces the bus and its slot the top edge, component side still up): the view's "up" is board -x, so the view's left = board +y: the adapter's pin-1 end is its board y-max end and the right-hand hole beside the power pads is its y-min hole (H2). standoff_placements.py holds the geometry (HX, adapter()).

J2 and the ribbon: straight, pin 1 to pin 1

A straight (untwisted) ribbon with its two plugs crimped alike joins two headers that are oriented alike: same pin-1 end, same key-slot side. The adapter's pin 1 is at its board y-max end, so J2's pin 1 is at its y-max end too. J2 = Connector_IDC:IDC-Header_2x20_P2.54mm_Vertical at rotation 180: pad 1 at the y-max end (square pad, "PIN 1" on the silk), the odd pins 1..39 in the row on the adapter side (+x: almost every CF signal is on an odd pin, so the CF chips beside J2 reach them directly), the even pins on the bus side, the shroud's key slot on the odd-row (+x) side. With standard 2-row numbering (the same on every box header and IDC plug: pin 2 across from pin 1 - on a board seen from above with pin 1 at the left end, pin 1 is in the lower row and pin 2 above it, like a Raspberry Pi header) this is the adapter's orientation, so the red stripe lies along the y-max end at both plugs and the ribbon arches up out of J2's plug and down into the adapter's, a translation only. gen_standoff.py check verifies that J2's pin 1 is at the adapter's pin-1 end and J2's odd row faces the adapter.

Pin 20. J2 is a full 2x20 (pin 20 fitted; JP2 can put +5 V on it for adapters powered through the header). A 40-way IDC plug with pin 20 open (generic 40-way IDC sockets are) fits both J2 and the adapter. A plug with pin 20 blocked (the keyed IDE cable kind) fits the adapter but not J2: use an open plug at the J2 end, or pull J2's pin 20 out of its header. JP2 stays in the design but OPEN by default: this adapter has no pin 20, so JP2 does nothing for it; it is harmless and serves other adapters.

Standoffs, holes and heights

  • H1 / H2: the adapter's two holes, 3.2 mm NPTH (MountingHole_3.2mm_M3, board-only footprints: not in the schematic, not in the BOM; the netlist proof accepts exactly these two, check_netlist.py is_mech()), each inside a 7 mm copper keep-out on all four layers (rule area: no track, no via, no plane fill: both planes pull back to 3.5 mm); no pad copper within 4.0 mm of a hole centre (the washer / nut on the bottom), no part body within 3.5 mm (the hex standoff on top); a silk circle where each standoff stands.
  • Proposed standoff: 15 mm M3 hex, female-female (5.5 mm across flats), with M3 x 6 screws and washers (or 15 mm male-female with a nut under the card). The adapter's underside is then 15 mm above the card; with its pin tails (~2-2.5 mm under it) that leaves ~3.5 mm over socketed DIPs (~8.5-9.5 mm). 12 mm standoffs lower everything by 3 mm but leave only ~0.5-1 mm over socketed DIPs.
  • Under the adapter only low parts: DIPs in sockets, disc caps, nothing else. gen_standoff.py check fails if anything tall (J2, J3, JP1, JP2, U$1 + jumpers, C30, the LEDs, X1) is under the adapter or under the ribbon.
  • Total height above the card (15 mm standoffs): adapter top 16.6 mm; CF holder + card (~8 mm) ~25 mm; the IDC plug on the adapter's header ~30 mm; the ribbon loop over it ~35 mm. Below the card: screw heads / nuts + washers ~3 mm (the solder tails already stand ~1.5-2 mm). Card cage: RESOLVED (2026-09-25) - nothing will be in front of the memory card: the slot on its component side stays empty, so the stack height does not matter (it was open question 4, "slot pitch vs ~35 mm stack").
  • The adapter hangs on its header end only (both holes are there); the CF slot end is free, ~29 mm past the holes. Inserting a card pushes toward the bus, i.e. into the standoffs, which is fine; if it wobbles, a stick-on bumper under the slot end (15 mm) would steady it.

The ROM stays removable (a constraint)

gen_standoff.py check enforces, on every option: the ROM IC13 and a keep-clear zone of 10 mm past both short ends and 2 mm along both long sides of its pads (lever it out; a 28-pin ZIF socket, ~50 x 15 mm, fits) hold no other part, and neither the ROM nor that zone comes within 3 mm of the adapter outline, a standoff or the ribbon zone. In A and B the ROM stands vertical at the free top edge (pads x 175.3 / 190.5, y 55.9-88.9; zone x 172.0-193.7, y 44.8-99.0 = print grid x 154.3-176.0, y 34.8-89.0): 44.8 mm from the adapter's slot edge, ~74 mm from the standoffs, ~80 mm from the ribbon, nothing above it, and the top edge is the part of the card reachable with the card in the cage. Its decoupling cap C3 moved beside its long side (outside the zone) so both short ends are clear.

Options A and B

Common to both: column 1 at the bus connector as in top-edge option B (the TMP registers IC27/IC29/IC26/IC28, the address buffers IC9/IC8, RN5/RN6); J2 pin rows at board x 76.17 (even) / 78.71 (odd) = print grid x 58.4 / 61.0 (target: ~59 +/- 10 from the bus edge); the adapter's header edge at x 83.19 (0.75 mm past J2's courtyard), its slot edge at x 127.19 (print grid x 65.4 / 109.4); both holes at board x 98.49 = print grid x 80.7; the CF column (IC30-IC34, horizontal DIPs, caps toward J2) right beside J2's odd row, three of its rows under the adapter's header half between the standoffs; the RAMs IC1/IC2 and IC5/IC15/IC11 in the column at x 122 (their left ends under the adapter's slot half); the block decode IC7/IC4 beside IC18 and the U$1 jumpers; IC6/IC12/IC10 vertical between the RAMs and the ROM; the ROM at the top edge; IC3 and the LED resistors R14/R2 near the LEDs. JP2 stands in the channel between column 1 and J2, beside J2's pin 20.

standoff-a: adapter centred standoff-b: adapter toward the y = 124 edge
adapter (board mm) x 83.19-127.19, y 36.85-96.85 x 83.19-127.19, y 63.52-123.52
adapter (print grid) x 65.4-109.4, y 26.8-86.8 x 65.4-109.4, y 53.5-113.5
H1 (pin-1 end) board (98.49, 92.85) = grid (80.7, 82.8) board (98.49, 119.52) = grid (80.7, 109.5)
H2 (power-pad end) board (98.49, 40.85) = grid (80.7, 30.8) board (98.49, 67.52) = grid (80.7, 57.5)
J2 pins y 42.72-90.98, pin 1 (78.71, 90.98) = grid (61.0, 81.0) pins y 69.39-117.65, pin 1 (78.71, 117.65) = grid (61.0, 107.6)
CF column IC32 / IC31 / IC34 between the standoffs (DA latch near J2 pins 33-37, strobes near 23-25, data buffer beside D0-D7), IC33 / IC30 past J2's pin-1 end IC33 / IC31 / IC34 between the standoffs, IC32 / IC30 below the y-min standoff; IC6 moves into the space J2 leaves at the y = 10 end
J3 (adapter power) + C30 J3 just outside the adapter's y-min edge beside H2 and the power pads (J3 at 93.98, 34.29), C30 beside it J3 just outside the adapter's y-min edge beside H2 (93.98, 60.96), C30 next to it
R10-R13 / RN9 at J2's y-min end / past its pin-1 end at J2's y-min end / in the channel beside J2
under the adapter IC31, IC32, IC34, the left ends of IC1, IC2, IC5, IC15 + caps IC31, IC33, IC34, the left ends of IC2, IC5, IC15, IC11 + caps
placement airwire 11,507 mm 11,698 mm
trial route 0 unrouted, 94 vias, 13,540 mm (F.Cu 7,521 / B.Cu 6,018) 0 unrouted, 100 vias, 13,748 mm (F.Cu 7,225 / B.Cu 6,523)
DRC copper violations 0 0

For comparison, the top-edge board (the record): airwire 10,496 mm, route 43 vias / 11,779 mm. J2 in the middle of the card is a wall every bus-side signal to the right half has to cross (the address and data buses to the memories, the decode lines), hence ~2x the vias and +15 % track; both routes are complete with 0.25 mm tracks and no copper violation, and the final polish (via clean-up, as on the top-edge board) would lower the count somewhat.

Recommendation: standoff-a. Shorter wiring and fewer vias, the adapter centred on the card (its standoffs 30.8 / 31.1 mm from the two side edges; in b H1 is 4.5 mm from the y = 124 edge), J3 and C30 at J2's y-min end right beside the adapter's power pads, and the y = 124 corner (LEDs) well clear of the adapter. b leaves the y = 10 half of the middle of the card free under the U$1 jumpers, at the cost of 6 more vias and the adapter's hole H1 near the board edge.

Trial route (both): Freerouting 1.9 on a two-signal-layer copy (planes carry GND/VCC), one run per pass count 20 / 30 / 40 / 60 in parallel (where Freerouting stops changes the result; all four agreed this time), the best kept (fewest unrouted, then vias, then length); the session imported onto the 4-layer board, planes refilled, DRC with schematic parity (options-standoff/reports/standoff-X-trial.txt, -trial-drc.json). Routability proof only: no clean-up, no silkscreen tidy (silk_overlap 41 cosmetic items: option boards).

Files per option X, all in options-standoff/ (since 2026-10-01; they were at the top level when the options were reviewed): memory-v2.0-standoff-X.kicad_pcb / .kicad_pro / .kicad_dru (the placement, unrouted), memory-v2.0-standoff-X-trial.kicad_pcb (+ .kicad_pro, .kicad_dru: the trial route), memory-v2.0-standoff-X-render-top.png (3D, the adapter drawn on the silk of a review copy), memory-v2.0-standoff-X-placement.png (outline, silk, adapter, ribbon zone, ROM zone, airwires), memory-v2.0-standoff-X-trial.png (the trial route: F.Cu red, B.Cu blue), memory-v2.0-standoff-X-1to1.pdf (below), options-standoff/reports/standoff-X-placement-check.txt, -drc.json, -trial.txt, -trial-drc.json, -freerouting.log.

The 1:1 check prints (memory-v2.0-standoff-a-1to1.pdf, -b-1to1.pdf)

US Letter, landscape, print at 100 % / "Actual size" (a 100 mm check bar on each page; also: the two hole crosses are 52.0 mm apart). Page 1: the board 1:1, component side up, bus-connector edge left, the JP1 end at the top; a 10 mm grid in mm from the bus-connector edge (x) and the JP1 end (y) - the same grid as the first fit print, whose "JP2 end" is this JP1 end; parts shaded, pads dotted; J2 highlighted with its pin 1; the adapter in place (blue: outline, its two holes with crosses and the standoff circle, header shroud and pins, its pin-1 end, the pin-20 column, the power pads (approx.), the CF slot edge); the ribbon zone; the ROM ("keep clear, removable") and its keep-clear zone; J3; the numbers (hole, J2, adapter, ROM zone positions in grid mm; standoffs; the trial route). Page 2: the side view at 1:1 (the height stack) and the notes (standoffs, total height, the card cage, pin 20, power). Every page is stamped with the date and time it was made. Made by print_1to1.py (system python3 + reportlab) from the geometry gen_standoff.py geom reads out of the board; build.sh regenerates both.

Open questions

  1. Pin 1 of the adapter's header: CONFIRMED (2026-09-24): a straight standard 40-pin ribbon, pin 1 to pin 1, joins J2 to the adapter as drawn (the adapter's pin 1 at the left end of its outer row, viewed component side up with the header at the top; the missing pin 20 is the 10th of the inner row from the left).
  2. ~~Adapter power pads~~ RESOLVED (2026-09-26): a 4-pin floppy (Berg) pinout, +5V / GND / GND / +12V, the same order as J3 (+5V, G, G, nc; pin 1 square), so the cable is straight through, pin 1 to pin 1, and the adapter never sees +12 V. The harness is made by hand; only the adapter's pin-1 pad is left to spot when making it.
  3. Ribbon: ~8-10 cm between the two plugs (the loop on page 2), 40-way, pin 20 open at the J2 plug (or J2's pin 20 pulled); plugs crimped alike, stripe on the pin-1 (y-max) end. Buy or crimp; the length is best tried with the print and the adapter on real standoffs.
  4. ~~Card-cage slot pitch vs. the stack height~~ RESOLVED (2026-09-25): nothing will be in front of the memory card (the slot on its component side stays empty), so the ~35-44 mm stack does not matter.
  5. Standoff length: 15 mm proposed; 12 mm if the sockets and the adapter's pin tails allow (measure the tails). The finished board uses 15 mm (the BOM's hardware lines).
  6. ~~Pick A or B~~ E chosen (2026-09-25), finished: "The v2.0 board" above.

The standoff options C / D / E: J2 and the adapter at the top edge (2026-09-24, later)

The brief: the IDE connector and CF card may move towards the top edge as long as the ROM stays uncovered - it might help reduce vias. Options A and B stay as they were (above); C, D and E keep the concept (J2 parallel to X1, just beside the adapter's header edge on the bus side; the adapter on two 15 mm M3 standoffs, header edge toward the bus, CF slot toward the free top edge; a straight ribbon; J3 beside the power pads; NPTH 3.2 mm holes in 7 mm keep-outs; only low parts under the adapter; the LEDs in the free top-edge corner; JP1 and the U$1 block jumpers as built) and move J2 and the adapter as far toward the top edge as they go: the CF slot edge 0.49 mm inside the top edge.

What it looks like on the card (read this first). J2 is the memory card's own 2x20 IDE header, soldered to this board. The CF adapter does not plug into J2: it sits 15 mm above the card on its two standoffs and has its own IDE header; a short 40-wire ribbon (~5-8 cm between the two plugs) runs up out of J2's plug and down into the adapter's plug, pin 1 to pin 1. The CF card goes into the adapter's slot at the top edge. Every drawing says so: J2 solid ("J2 - IDE HEADER ON THIS BOARD", pin 1 = the square pad), the adapter's header dashed ("ADAPTER'S IDE HEADER (on the adapter, 15 mm above)"), grey arrows for the ribbon ("SHORT 40-WIRE RIBBON, pin 1 to pin 1"), the thick slot edge "CF CARD INSERTS HERE (into the adapter)"; the 1:1 prints add numbered callouts and a side view with J2 and its plug, the ribbon loop, the standoffs, the adapter with its header and plug, and the CF card in its holder.

J2's plug envelope (new rule, 2026-09-24; C, D, E)

J2 with an IDC ribbon plug on it stands ~18 mm above the card (shroud ~9 + plug ~9), higher than the 15 mm standoffs, and the plug body is ~1-1.5 mm wider than the shroud on each side. So J2's plug envelope = its shroud + 1.5 mm all round, 18 mm tall, and gen_standoff.py check requires (constants in standoff_placements.py: PLUG_SIDE, PLUG_H, J2_SHROUD_GAP):

  • the envelope entirely outside the adapter outline, and the adapter's header edge 3.0 mm from J2's shroud (target: ~3-5 mm, so the ribbon can fold up out of J2's plug and down into the adapter's plug on the adapter's header, ~15 + 1.6 + 9 mm up); on C, D, E the envelope ends 1.5 mm before the adapter (x 149.54 / 151.04). The next grid step (4.27 mm) would cost column 3 another 1.27 mm;
  • no other part's body inside the envelope (on the bus side too: the plug body overhangs socketed DIPs there).

A and B predate the rule and do not meet it (J2's shroud 1.19 mm from the adapter's header edge, the envelope 0.31 mm under the adapter): the check prints that as a NOTE for them. If A or B is picked, the adapter moves 1.81 mm toward the top edge (or J2 1.27 + 0.54 mm toward the bus) and the card is routed again.

The ribbon. Straight up out of J2's plug (top ~18 mm), a loop ~6 mm above the adapter's plug (top ~35 mm), down into it: ~4 cm is the minimum between the two plugs (standoff_placements.ribbon_length(): 37 mm for C/D/E, 35 mm for A/B), 5-8 cm is comfortable to plug and unplug with the adapter on its standoffs. 40-way, plugs crimped alike, pin 20 open at the J2 plug (as before). Heights: J2 + plug ~18, CF card top ~22, the adapter's plug ~35, the ribbon loop ~42 mm above the card (page 2 of the prints).

The layout of C, D and E

The card flows as the top-edge board did (43 vias): X1 | column 1 (TMP registers IC27 / IC29 / IC26 / IC28, the address buffers IC9 / IC8, RN5 / RN6; as before) | column 2 (glue, x 74.93) | column 3 (the memories, x 102.87) | J2 | the adapter over the CF chips. J2's odd row at x 144.75 (the last 1.27 mm grid column that keeps the slot edge on the board), the adapter x 151.04-195.04 (print grid 133.3-177.3), slot edge 0.49 mm inside the top edge; both standoff holes at board x 166.34 = print grid 148.6. J2 is no longer a wall between the bus and the memories: only the CF section's own lines (DATA0-7, IO-ADDR0-3, the strobes, reset: ~15 nets) pass it, round its ends or between its pins. Column 3 closes up 6.35 mm against the top-edge board (its 28-pin bodies end at x 137.1, J2's plug envelope starts at 137.4); column 2 1.27 mm. Under the adapter (all sockets, disc caps, axial resistors): its header half, between the standoffs, holds IC32 (DA latch, beside J2 pins 33-36), IC31 (strobes, beside 23 / 25) and IC34 (data buffer, beside D0-D7 = pins 3-17, the pin-1 end); its slot half holds IC33 beside the pin-1-end standoff H1, IC4 beside H2 (C, D), the pull-ups R10-R13 and RN9. J3 just outside the adapter's y-min edge beside the power pads (and H2).

They differ in where the ROM goes (IC13 shares 23 bus lines with the RAMs IC1 / IC2, and needs to stay uncovered):

standoff-c: ROM at the top edge beside the adapter standoff-d: ROM in the memory column, bottom row standoff-e: ROM in the memory column, top row
idea the proposed example: the ROM horizontal at the free top edge between the adapter and the LEDs the ROM with the RAMs (IC15, IC1, IC2, ROM top to bottom), below J2's pin-1 end the ROM with the RAMs (ROM, IC1, IC2, IC15), under the U$1 jumpers, above J2's pin-39 end; J2 and the adapter toward the LED side
J2 (board mm) pins y 35.10-83.36, pin 1 (144.75, 83.36) = grid (127.0, 73.3) same as c pins y 61.77-110.03, pin 1 (144.75, 110.03) = grid (127.0, 100.0)
adapter (board / grid) x 151.04-195.04, y 29.23-89.23 / x 133.3-177.3, y 19.2-79.2 same as c x 151.04-195.04, y 55.90-115.90 / x 133.3-177.3, y 45.9-105.9
H1 (pin-1 end) board (166.34, 85.23) = grid (148.6, 75.2) same as c board (166.34, 111.90) = grid (148.6, 101.9)
H2 (power-pad end) board (166.34, 33.23) = grid (148.6, 23.2) same as c board (166.34, 59.90) = grid (148.6, 49.9)
ROM IC13 + keep-clear zone horizontal at the top edge, pads x 158.1-192.4, y 94.8-112.5; zone x 148.1-195.5 (+ air past the edge), y 92.8-114.5 = grid x 130.4-177.8, y 82.8-104.5; 4.6 mm from the adapter horizontal, pads x 102.2-136.5, y 94.8-112.5; zone x 92.2-146.5, y 92.8-114.5 = grid x 74.5-128.8, y 82.8-104.5; 5.8 mm from the adapter horizontal, pads x 102.2-136.5, y 33.9-51.6; zone x 92.2-146.5, y 31.9-53.6 = grid x 74.5-128.8, y 21.9-43.5; 5.1 mm from the adapter
block decode IC7 / IC4, port decode IC30 IC7 in the JP1 top-edge corner, IC4 under the adapter; IC30 in column 3 (bottom) IC7 in the corner, IC4 under the adapter; IC30 past J2's pin-1 end below the adapter IC7, IC4, IC30 in the JP1 top-edge corner beside the U$1 jumpers (as on the top-edge board)
placement airwire 12,024 mm 10,974 mm 11,118 mm
trial route (best of 8 orders) 0 unrouted, 82 vias, 14,096 mm (F.Cu 7,768 / B.Cu 6,328) 0 unrouted, 77 vias, 12,502 mm (F.Cu 7,175 / B.Cu 5,326) 0 unrouted, 72 vias, 12,579 mm (F.Cu 7,042 / B.Cu 5,537)
its 8 orders 4 complete (82-98 vias), 4 with 1-2 left 4 complete (77-84 vias), 4 with 1 left 7 complete (72-85 vias), 1 with 1 left
DRC copper violations 0 0 0

For comparison: A 94 vias (committed trial; 8 new orders of its committed board: 88-111 vias, 2 of 8 incomplete), B 100, the top-edge board 43 (airwire 10,496 mm).

How the trials were routed (changed for C, D, E). Freerouting 1.9 repeats itself for one input file: the pass limit changes nothing (it stops by itself; A's four pass counts all agreed), and neither does the order of the nets. The order in which the DSN lists the components does change the route, by +/- 15 vias for the same placement. So each option is now routed in 8 component orders (gen_standoff.py shuffle, SEEDS in build.sh, seed 0 = as exported) in parallel and the best is kept (fewest unrouted, then vias, then length); the order kept is in options-standoff/reports/standoff-X-order.txt. A and B keep their trials of the earlier method (records). One more lesson from the trials: placement details matter at this density - D's first placement (ROM, IC15 and the RAMs in another order, IC5 two rows higher) never completed in 17 orders (BDATA5 / BDATA7 at the RAMs); putting the RAMs next to the ROM and IC5 beside them fixed it and cut the airwire to the lowest of all options. A fourth arrangement, the ROM at the top edge in the JP1 corner with the adapter toward the LEDs, routed worst (113 vias) and was dropped.

Recommendation: standoff-e (chosen 2026-09-25: "The v2.0 board" above)

  • Fewest vias and the most robust route: 72 vias, -23 % against A (94) and -18 % against A's best new order (88); 7 of its 8 route orders complete, all within 72-85 (C and D: 4 of 8). Track 12,579 mm (A 13,540).
  • The ROM with the RAMs, uncovered, in the top row of the memory column under the U$1 jumpers: 23 bus lines short, and its keep-clear zone 5.1 mm from the adapter, clear of J2, the ribbon and the standoffs.
  • The block decode IC7 / IC4 and the port decode IC30 back in the JP1 top-edge corner beside the jumpers they serve (as on the top-edge board), not under the adapter.
  • J2 and the adapter toward the LED side leave that JP1-end corner free for them; the adapter ends 1.0 mm short of the LEDs' bodies (H1 12.1 mm from the y = 124 edge), J2's shroud ~9 mm from it with JP2 just past its pin-1 end.
  • Cost: the ROM is no longer at the top edge (it is pulled with the card out of the cage, like the RAMs).

D is the close second: the lowest airwire of all (10,974 mm) and the shortest route (12,502 mm), 77 vias, but only half its route orders complete; its ROM sits at the bottom of the memory column. C (the proposed example: the ROM at the top edge beside the adapter) keeps the ROM reachable in the cage but routes worst of the three (82 vias, 14,096 mm): the 23 ROM-RAM lines have to go round J2's pin-1 end to the top edge. None gets near the top-edge board's 43: J2 still stands between X1 and the CF chips (~15 lines cross it), the memory column gave up 6.35 mm to J2's plug envelope, and the standoff keep-outs sit in the CF section; the final polish (via clean-up) would take a few more off.

The 1:1 check prints of C, D, E

memory-v2.0-standoff-{c,d,e}-1to1.pdf, as for A and B (US Letter landscape, 100 % / "Actual size", 100 mm check bar, the holes 52.0 mm apart; the same grid: x from the bus-connector edge, y from the JP1 end). Page 1 now also marks J2 as the header ON THIS BOARD (solid, thick outline, "pin 1" with the square), its plug envelope (dashed red), the adapter's own header (dashed blue, "on the adapter, 15 mm above"), the ribbon (grey arrows) and the slot edge ("CF CARD INSERTS HERE"), with four numbered callouts under the board; page 2 is the side view described above. The A and B prints were remade with the same drawing (their placements and trial routes are unchanged).

Open questions, C / D / E

  1. ~~Pick one~~ E chosen (2026-09-25); routing polish, silkscreen tidy and fab files done: "The v2.0 board" above.
  2. The J2-to-adapter gap: 3.0 mm from J2's shroud to the adapter's header edge (the plug envelope 1.5 mm clear). If the real plug or the ribbon fold needs more, the next step is 4.27 mm (column 3 moves 1.27 mm toward the bus).
  3. ROM access (C / D / E): in C the ROM is at the top edge (reachable with the card in the cage); in D and E it is in the memory column, uncovered, pulled with the card out of the cage.
  4. The earlier open questions (pin 1 is confirmed; the power-pad order, the ribbon, the standoff length) hold for C, D, E too; the slot pitch (~44 mm with the plug on the adapter) is resolved: nothing in front of the memory card (2026-09-25).

The top-edge record: the board finished from option B (options-top-edge-J2/)

Superseded by the standoff decision the same day; kept as a record. Everything in this section and the next few (the finished board, its fab outputs, "Before ordering", the three top-edge re-layout options, their trial routes) was moved unchanged into options-top-edge-J2/ (reports: options-top-edge-J2/reports/); the file names below are in that folder. options-top-edge-J2/memory-v2.0.kicad_pro / .kicad_dru (the re-layout rules, as option B's) open the finished board with its rules. build.sh still re-checks it (step 5: DRC, finish_v2.py verify, the netlist proof); FROM=trial / ROUTE=1 remake it and its fab outputs there, RELAYOUT= the options.

options-top-edge-J2/memory-v2.0.kicad_pcb (until the standoff decision it sat beside the schematic, sharing memory-v2.0.kicad_pro, which still carries the re-layout rules). Made by finish_v2.py make from option B's committed trial route (memory-v2.0-relayout-b-trial.kicad_pcb, Freerouting 1.9 of 2026-09-24): FROM=trial build.sh remakes it exactly.

Which route. The committed trial route was compared with fresh routes of the same placement: eight new Freerouting runs (the trial's settings and lower optimisation thresholds, -oit 100 / 10 / 2 / 0.5) all came out at 61 vias, 11,887 mm and 1 connection left unrouted (DATA12 at IC29; the machine was heavily loaded, so the optimiser had far less time than the trial's). The trial route is better on every count (43 vias, 11,779 mm, complete), so it is the base.

Clean-up pass (finish_v2.py cleanup): - Vias: the Specctra session import had marked all 43 vias "buried" (F.Cu to B.Cu on a 4-layer board). They are now through vias (0.8 / 0.4 mm), the planes refilled around them. Fixed at the source too: gen_relayout.py ses converts them on import. The committed trial boards of 2cae926 still carry the buried type (a record, not remade). - Needless vias: for each via, the run of track on one side (up to the pad or via it ends on) was tried on the other signal layer, keeping the 0.2 mm clearance, the edge distance and every T-junction; the via goes if one layer is left. None could go: on every one of the 43 the run would cross another net's track on the other layer (Freerouting's optimiser had already removed the easy ones). 43 vias stay. - Collinear segments of one net / layer / width meeting end to end with nothing else at the joint were merged (1,801 -> 1,794 segments; no geometry change). No jog worth removing was found: the optimiser pulls tracks tight.

Placement changes after the pick (the only ones; every other part is exactly where option B has it): - C20-C23 taken off (2026-09-24): finish_v2.py make drops their footprints (drop_removed()) after the silkscreen tidy, so no other text moves because of them, then refills the planes. Their pads were plane-only (GND / VCC through thermal reliefs): no track or via touched them, none was removed, the routing is unchanged (43 vias, 1,794 segments, 11,779 mm). Made on the committed board: the result is the previous board minus exactly the four footprints (their references with them) and the two refilled plane zones; FROM=trial build.sh gives the same board (only the UUIDs of the texts make adds differ). - C30 (10 uF, adapter power) moved 2.54 mm inboard (away from the top edge, x 185.42 -> 182.88, y 22.86 unchanged): frees the row left of J3 pin 1 for its "+5V" label. Its two pads are plane-only (GND / VCC), no track moved. - The LEDs stay where option B has them (PWR0 at 191.74 / 120.19, LED1 ACT at 182.88 / 120.19, the free top-edge corner at y = 124, beside the adapter's end): nothing collides with them.

Silkscreen (finish_v2.py make, checked by finish_v2.py silk / verify and the DRC): - Board title "YACC1 MEMORY BOARD V2.0" (the built card's title text, same place); "onepagecomputer.com" kept. - "CF: P8/P9" just past the y = 124 end of J2's shroud; J2's pin-1 triangle from the library. - J3 pin labels, one per pin, left of the pins: +5V, G, G, nc (pin 1 = +5V, square pad). - JP2 "PIN20 +5V" beside the jumper (IDE pin 20 = +5 V for adapters powered through the header). - The block-removal jumper group labels as on the built card: ROM / RAM / 0X8000 / 0XF000 at U$1, the "1" pin marks of RN7 / RN8; the bus-enable jumper JP1 "-BUS-EN" above it and "Gnd" (the built card has "Gnd" above pin 3, where it ran into "-BUS-EN"; now beside pin 3). - LED labels "PWR" and "ACT" above the two LEDs. - Reference texts: every IC's reference in the middle of its body (its value on F.Fab just below, for the placement PDF); every other reference beside its part. 46 texts were moved by the tidy (most 0.3-0.5 mm off their own outline, the largest LED1 5.1 mm, C8 3.1 mm, C24 / PWR0 2.6 mm; four of the 46 were C20-C23's, which went with their parts), R2's upside-down reference turned upright, the U$1 reference thickened to 0.15 mm. Result: no reference or board text touches a pad, a via, other silk or the edge, none is upside down (reports/memory-v2.0-final.txt); DRC silk_overlap 0 (the built card: 45). - F.Fab keeps the TAODAN CF-IDE40 outline: the 70 mm adapter strip (solid) and the keep-low zone (dashed) around J2, with a note; F.Fab is on the placement PDF, not on the gerbers.

Final numbers (reports/memory-v2.0-final.txt, -drc.json, -drc.rpt)

v2.0 final board the built card v1.3 (its own rules)
unrouted 0 0
vias 43, all through, 0.8 / 0.4 mm (built: 0.4572 / 0.254 mm)
track 1,794 segments, 11,779 mm (F.Cu 6,858 / B.Cu 4,921), all 0.25 mm; placement airwire 10,496 mm 1,377 tracks and vias, 0.1524 mm
DRC copper violations 0 (clearance, shorts, width, via, hole, edge, starved thermal, dangling, unconnected) 0
planes GND on In1.Cu and VCC on In2.Cu each one piece, ~16,500 mm2 (81-82 % of the board after antipads); all 174 GND/VCC pads on their plane through thermal reliefs (182 before C20-C23 went) same stack-up
DRC items left, all inherited X1's two mounting holes in X1's own keepout 2/2, X1 library mismatch 1/1, X1 silk over the edge 4/4, X1 pin-number text height 2/2, Eagle-footprint silk outlines over pads (silk_over_copper) 199/199
DRC silk_overlap / text_thickness 0 / 0 45 / 1
schematic parity 49 items, all the built card's inherited Eagle values/fields (53 before C20-C23 went: four were theirs); new: none 220
ERC 99 (= the built card's 104 residue - 6 bus labels now global + the designed-in SRST label; removing C20-C23 changed nothing), PASS 104
netlist proof MATCH (70 parts, 186 nets, 687 pads)
placement check OK (no overlap, pads 0.5 mm inside the edge, X1 as built, TAODAN keep-low zone clear)

Fab outputs (finish_v2.py fab; remade only by a FROM=trial / ROUTE=1 build)

File What
memory-v2.0-gerbers.zip the upload: the 12 files of gerbers/
gerbers/memory-v2.0-F_Cu.gbr, -In1_Cu.gbr, -In2_Cu.gbr, -B_Cu.gbr copper L1 (signals) / L2 (GND plane) / L3 (VCC plane) / L4 (signals)
gerbers/memory-v2.0-F_Mask.gbr, -B_Mask.gbr, -F_Silkscreen.gbr, -B_Silkscreen.gbr, -Edge_Cuts.gbr masks, silkscreens (the bottom one is empty), outline
gerbers/memory-v2.0.drl, -drl_map.gbr, -job.gbrjob Excellon drill (plated and non-plated in one file, mm), drill map, Gerber job file (4 layers, 1.6 mm)
memory-v2.0-jlcpcb-order.txt the order parameters, as the built card's JLCPCB order 2000765A-Y42 (../../eagle/v1.3/fab/jlcpcb-order-2000765A-Y42.zip, YG/4te.json): FR-4, 4 layers, 1.6 mm, outer copper 1 oz, inner 0.5 oz, green mask, white silk, HASL with lead, vias plugged
memory-v2.0-render-top.png, memory-v2.0-render-bottom.png 3D renders
memory-v2.0-placement.pdf assembly drawing: silkscreen + F.Fab (values, the TAODAN outline) + outline, title block
memory-v2.0-schematic.pdf, memory-v2.0-bom.csv schematic (7 sheets), BOM (35 lines, 70 parts)

Before ordering (the top-edge board; superseded by the standoff decision)

  1. J2 pin 1 / key vs the adapter. J2 (shrouded 2x20, rotation 0) has pin 1 toward y = 10, the odd pins inboard (x = 189.20); check on which side of the shroud the library's key slot falls. TAODAN CF-IDE40: it plugs straight onto J2 and stands perpendicular to the card, out of the component side; its socket's pin 1 decides which way its board then faces (components toward the card or away). Check against the adapter in hand: a 180 degree turn of J2 would put the odd pins outboard and cost a re-route. SinLoon on a ribbon: only the cable's key/twist matters.
  2. J3 pinout (1 +5 V, 2/3 GND, 4 n/c, the CF card v1.0's) against the adapter's floppy-style power cable.
  3. Socket heights under a TAODAN overhang: nothing tall and no IC is inside the keep-low zone, but IC34 is 5.4 mm from it (J3 5.2 mm, the LEDs 6.3 mm); sockets + chips are ~8-9 mm tall, the adapter's lower edge ~9-10 mm up. Measure the adapter.
  4. Which backplane slot: the TAODAN needs ~75 mm free on the card's component side, i.e. the neighbouring slot on that side empty (or use a SinLoon on a ribbon).

Decided: C20-C23 (the built card's four 100 nF with no IC beside them, kept until then as spare plane-to-plane decoupling): removed (2026-09-24, the unused capacitors on the memory card); schematic, board and fab files re-made (part-list delta above).

Not ordered.

The re-layout (2026-09-24; the rules and stack-up hold for the standoff options too)

Kept from the built card: the board outline (177.8 x 114.0 mm, x 17.72-195.55 / y 10.00-124.02), the bus connector X1 (FABC96R, same position and orientation, its two mounting holes and keepouts: the card plugs into the same backplane; there are no card guides in the cage) and the 4-layer stack-up: In1 = solid GND plane, In2 = solid VCC plane (the built card's plane outlines), signals on F.Cu and B.Cu only. Discarded: every one of the built card's 1,377 tracks and vias, and the placement of every part but X1. All parts through-hole, no SMD.

Orientation. The card stands on X1 in the cage, so board +x is UP: the x = 195.55 edge is the free top edge (J2 goes there), y = 10 and y = 124 are the two free side edges. The block-map jumpers U$1 and JP1 stay at the y = 10 side edge where the built card has them; the LEDs, JP2 and J3 sit at the top edge.

Power. No power track anywhere: every GND/VCC pin (ICs, caps, headers, X1's six + six supply pins) is a through-hole pad that reaches its plane through a thermal relief (0.4 mm gap, 0.5 mm spokes; antipads 0.3 mm). The DRC's "0 unrouted" of the trial boards includes every power pin reaching its plane. Decoupling: one 100 nF per IC, standing beside the IC's pin-1 / VCC end (the built card's arrangement): C1-C19, C24 for the built card's 20 ICs (same pairs as built), C25-C29 for the CF chips; C30 (10 uF) at J3. C20-C23 (the built card's four caps with no IC beside them) were placed in the options as plane-to-plane decoupling (C20/C21 at X1's two power groups, C22/C23 at the far end of the planes) and then removed from v2.0 (2026-09-24): they are on the option boards and trial routes (made before), not on the final board.

Design rules (memory-v2.0.kicad_pro and memory-v2.0-relayout-X.kicad_pro net classes + .kicad_dru)

re-layout the built card
signal track width 0.25 mm (10 mil), every trial-route track 0.1524 mm (6 mil)
clearance 0.2 mm (8 mil) 0.127 mm, Eagle 0.4572 mm track-track, 0.254 mm track-pad
vias 0.8 / 0.4 mm (pad / drill) 0.4572 / 0.254 mm
copper to board edge 0.5 mm 0.381 mm
hole to hole / hole clearance 0.5 / 0.25 mm 0.254 / 0.127 mm
power net class Power (GND, VCC): not routed, planes only same planes
planes clearance 0.3 mm, thermal gap 0.4 mm, spoke 0.5 mm 0.2 mm spokes

With these rules one 0.25 mm track fits between two X1 pins, one between two KiCad DIP pins (1.6 mm round pads) and two between two pins of the Eagle DIL footprints the built card's parts keep (1.22 x 2.44 mm oval pads). The track pitch (0.45 mm) is finer than the built card's effective 0.61 mm (6 mil tracks at its 18 mil Eagle spacing), so the re-layout is no harder to route than the built card was; only the vias are bigger.

Placement grid and footprints

Every pad of the card is on one 1.27 mm grid, the grid of X1's pins (anchor X1 A1 = 22.83, 106.22). The built card's parts keep their converted Eagle footprints (the netlist proof requires the schematic's footprints); the CF parts use the KiCad standard libraries as on the CF card v1.0. ICs are in columns of horizontal DIPs (pin 1 bottom left, as on the built card), row pitch 13.97 mm, 5-8 mm channels between columns. J2 (Connector_IDC:IDC-Header_2x20_P2.54mm_Vertical, shrouded, pin 20 present) is at rotation 0 in every option: pads at x = 189.20 (odd pins, inboard: almost every IDE signal is on an odd pin) and 191.74, shroud 0.6 mm inside the top edge, pin 1 toward y = 10.

Top-edge placement options (the review; B was chosen; now the record in options-top-edge-J2/)

Every option: same circuit (netlist proof MATCH, board and trial route; made before C20-C23 were removed, so every option board, trial route and keep-copper record still carries them: see "The records and C20-C23" below), no body overlap, every pad 0.5 mm inside the edge, X1 exactly as built, the TAODAN keep-low zone (12 mm past each end of J2's pin row, 7 mm either side of its centre line) holding no IC and nothing tall (reports/relayout-X-placement-check.txt). Column 3 is the memories (IC1 low RAM, IC2 high RAM, IC13 EEPROM) under the block-map jumper group, which keeps the built card's exact pad positions (RN7, U$1, RN8, IC18, C24; its ROM / RAM / 0X8000 / 0XF000 labels move with U$1). Column 1 is next to X1.

idea J2 (top edge) / adapter overhang LEDs, JP2, J3
A the built card's topology, re-flowed: col 1 bus side (IC14, IC6, IC5, IC9, IC3, IC8, RN5/RN6), col 2 decode (IC7, IC4, IC15, IC11, IC12, IC10, IC30), col 3 memories + IC31, col 4 TMP registers IC26-IC29 above the CF chips IC34, IC32, IC33 lower half, pins y 64.3-112.6; strip y 53.4-123.4 PWR, ACT, JP2, J3 in the other top corner (y = 10 side)
B TMP registers IC27/IC29/IC26/IC28 right at the bus connector (they use nothing but the data bus and four strobes, all entering at X1's upper half), address buffers IC9/IC8 below them; col 2 strobes, data buffer IC5, FORCE-ROM glue; col 3 memories + IC15; col 4 = the CF column (IC7/IC4 at its top beside IC18 and the jumpers, then IC33, IC34, IC31, IC32, IC30) with RN9 and R10-R13 between it and J2 centred, pins y 50.3-98.6; strip y 39.5-109.5 PWR LED where the built card has it (y = 124 corner), ACT beside it; JP2, J3, C30 at the y = 10 corner
C option A's columns 1-3; column 4 turned round: CF chips IC33, IC34, IC32 at the top, TMP registers below upper half, pins y 21.1-69.4; strip y 10.3-80.3 PWR LED where built, ACT beside it, JP2/J3 between them and J2

Trial autoroute (build of 2026-09-24)

Freerouting 1.9 on a two-signal-layer copy of each board (planes dropped, class Power not routed, 30 passes, one optimisation pass -oit 100, one thread), the session imported back onto the 4-layer board, planes refilled, DRC with schematic parity under the re-layout rules. This proves routability only: no finisher, no clean-up, no silk tidy. Freerouting is not deterministic: a new run gives other numbers (the previous full build, same placements but for a few silk labels, C22 in A and LED1 in B: A 0 unrouted / 47 vias / 12.8 m, B 0 / 45 / 11.9 m, C 0 / 40 / 12.5 m).

airwire (placement, MST of the 146 signal nets) unrouted after Freerouting vias total track length (F.Cu / B.Cu) DRC copper violations Freerouting time
A 11,438 mm 0 43 12,873 mm (7,004 / 5,869) 0 90 s
B 10,496 mm 0 43 11,779 mm (6,858 / 4,921) 0 125 s
C 11,173 mm 0 43 12,429 mm (7,409 / 5,019) 0 97 s

Every trial board: all tracks 0.25 mm; DRC copper violations 0 (clearance, shorts, track width, via size, hole clearance, edge clearance, starved thermals, dangling items, unconnected); the only non-cosmetic DRC items are X1's two mounting holes inside X1's own via keepout, which the built card's DRC has too; the rest is silkscreen and the Eagle library texts (reports/relayout-X-trial.txt, -trial-drc.json). Schematic parity: the built card's 53 inherited Eagle value/field items, nothing new.

Images per option: memory-v2.0-relayout-X-render-top.png (3D, the TAODAN strip solid and the keep-low zone dashed on the silk of a review copy), memory-v2.0-relayout-X-placement.png (2D: outline, silk, adapter zones, airwires), memory-v2.0-relayout-X-trial.png (the trial route: F.Cu red, B.Cu blue).

Recommendation: option B (chosen 2026-09-24)

  • Shortest wiring: the lowest airwire (-8 % against A) and the shortest trial route (11.8 m against 12.4-12.9 m) at the same via count. The TMP registers, the part that sank the keep-the-copper attempt, sit where their only signals enter: the 16-bit data bus and the four TMP strobes come straight off X1's upper half into them, and DATA0-7 continues in one bundle through IC5 to the CF buffer IC34 / latch IC32.
  • The CF section is one column at the top edge with its passives between it and J2, ordered by J2's pin sequence (IC33 reset/enable, IC34 data, IC31 strobes, IC32 DA0-2, IC30 decode nearest the IO-ADDR pins).
  • J2 centred on the top edge: the TAODAN's 70 mm board stays 29.5 / 14.5 mm inside the two side edges, the keep-low zone is clear of everything tall with 5 mm to spare, and a SinLoon ribbon leaves straight off the top edge.
  • The PWR LED stays where the built card has it; ACT is next to it; both visible from the top edge; JP2 (pin-20 power) and J3 (adapter power) are at the other end of the top edge, reachable with the card in the cage and outside the adapter overhang.
  • Cost: IC7 and IC4 (block decode) sit at the top of the CF column, ~35 mm from the U$1 jumpers they serve (the trial route runs them along the y = 10 side without trouble); IC15 is alone under the memories.

A is the most familiar (the built card's column order) but the longest; C has the same topology as A with the CF chips at the top and leaves the adapter strip 0.3 mm inside the y = 10 edge.

The CF-to-IDE adapter (the top-edge options; superseded: the HX-2118P on standoffs, above)

  • TAODAN CF-IDE40 V2.0 (70 x 63 mm, female 40-pin socket along a 70 mm edge) plugs straight onto J2 and stands perpendicular to the card, out of the component side, its lower edge ~9-10 mm above the card, overhanging each end of the 50.8 mm pin row by ~10 mm; +5 V from IDE pin 20 through JP2, or by cable from J3. Each option draws on User.Drawings (and on the silk of the render copy) the adapter strip (solid, 70 x 8 mm) and the keep-low zone (dashed): nothing taller than ~8 mm within 12 mm of either end of the pin row, and nothing tall within 7 mm of the header centre line (both sides: which way the adapter board faces is not known until it is in hand).
  • The card needs free space on its component side when the TAODAN is used (~75 mm): see "which slot" below.
  • SinLoon CF-to-IDE (60 x 43 mm, male 40-pin) on a short ribbon: J2 is shrouded and at the free top edge.

Open items at the review (superseded)

The list that went with the three options is now "Before ordering" above; its last point (the final routing polish, silkscreen tidy and fab outputs after the pick) is done.

The records and C20-C23

C20-C23 were removed (2026-09-24) after the re-layout options, their trial routes and the keep-copper options were made. Least churn: those nine boards and their renders, plots and reports are left as they were, documented as pre-removal records, not re-made. They carry the four caps exactly as the built board has them (same footprint, value, symbol path; pin 1 GND, pin 2 VCC); check_netlist.py --records checks each against the schematic + exactly those four, and build.sh accepts the four as "extra footprint" parity items on them (parity_new ... record) and on nothing else. Regenerating them (RELAYOUT= / KEEPCOPPER=) reproduces the same pre-removal records (gen_relayout.py board and gen_mem_v2.py board keep the four from the built board; checked with RELAYOUT=b NOROUTE=1 KEEPCOPPER=b on a scratch copy: BUILD PASS). Made without them: the top-edge finished board (finish_v2.py make takes them off, also after ROUTE=1, which routes option B's board with them on it) and the standoff boards (gen_standoff.py board leaves them off; made after the removal).

The keep-the-built-copper record (options-keep-copper/)

The three options of 4365de6 (the CF section added to the built card with all 1,377 built tracks and vias kept), moved here unchanged with their renders, plots and reports. None is legal: every one puts CF pads on the built card's DATA8-15 bundle (DRC: A 11 shorts / 4 clearance / 63 mask bridges, B 12 / 1 / 50, C 12 / 3 / 63), and space_check.py found no legal spot for all five CF DIPs (best packing 4 of 5, options-keep-copper/reports/space-check.txt, options-keep-copper/memory-v2.0-free-space.png). Regenerated only on request: KEEPCOPPER="a b c" build.sh (placements.py, gen_mem_v2.py board/locked/check, space_check.py).

Files

File What it is
mem_v2_netlist.py the delta (single source): CF card v1.0 -> v2.0 reference map, dropped parts, shared nets, check(), expected()
gen_mem_v2.py writes the schematic (sch; sheet 7 wired by tools/kicad/sch_wire.py); the board's schematic links (link); the keep-copper record boards (board, locked, check); refill, review (review images)
standoff_placements.py the standoff options A-E (plain data): the HX-2118P's measured geometry (HX, adapter()), J2's orientation and plug envelope (j2(), j2_geom(), PLUG_SIDE, PLUG_H, J2_SHROUD_GAP), ribbon_length(), the standoff / hole / ROM clearance figures; C-E's shared layout (cf_under(), j3_c30())
gen_standoff.py the standoff boards (board: placement, H1/H2 + keep-outs, the adapter / J2 / ribbon / slot drawings and labels), check (the placement gates above, J2's plug envelope), geom (for the print), shuffle (a DSN in another component order: the trial routes are the best of 8 orders); dsn / ses / stats / airwire / review = gen_relayout's
print_1to1.py the 1:1 US-Letter check print (reportlab, system python3) from gen_standoff.py geom
relayout_placements.py the top-edge re-layout options (plain data + helpers: row() = a DIP and its cap, j2(), labels(); the standoff options reuse row(), col(), UBLOCK_BUILT)
gen_relayout.py top-edge re-layout boards (board, into options-top-edge-J2/), check, airwire, trial route (dsn two-signal-layer export, ses import, stats); write_project() = the re-layout rules
finish_v2.py the v2.0 board: make-e (from a route of standoff E: through vias, via clean-up, collinear merge, the fab silkscreen, title block, refill), verify, fab-e (gerbers, NPTH/PTH drill, zip, renders, placement PDF, order note) + drill-check, bom-hw (H1/H2 + the hardware lines into the BOM); project (the v2.0 project gets the re-layout rules); for the top-edge record make, silk, fab
check_netlist.py the netlist proof: schematic = built v1.3 - C20-C23 + CF section; the standoff boards, their trial routes and the top-edge finished board = the schematic (+ the two board-only standoff holes H1/H2, is_mech()); the record boards (--records) = the schematic + exactly C20-C23 as on v1.3
build.sh the whole pipeline; exit 0 = every gate passed
memory-v2.0.kicad_sch, -sheet1..7.kicad_sch, .kicad_pro, .kicad_dru schematic (sheets 1-6 built v1.3, sheet 7 CF), project with the re-layout rules (shared by the v2.0 board)
memory-v2.0.kicad_pcb THE v2.0 BOARD (standoff option E, routed, finished; ordered from JLCPCB 2026-10-09)
memory-v2.0-gerbers.zip, gerbers/, memory-v2.0-jlcpcb-order.txt, memory-v2.0-render-{top,bottom}.png, memory-v2.0-placement.pdf, memory-v2.0-1to1.pdf its fab outputs ("Fab outputs" above)
options-standoff/ the standoff record (moved out of the top level 2026-10-01): the five options memory-v2.0-standoff-{a,b,c,d,e}.kicad_pcb / .kicad_pro / .kicad_dru (placed, unrouted, re-layout rules), their trial routes -trial.* (E's is what the v2.0 board was made from), the 1:1 check prints -1to1.pdf, the images -render-top.png (3D with the adapter), -placement.png (placement / airwires), -trial.png (trial-route copper); reports/ per option standoff-X-placement-check.txt, -drc.json, -trial.txt, -trial-drc.json, -freerouting.log (C-E also -order.txt). build.sh still re-checks every one of them
memory-v2.0-schematic.pdf, memory-v2.0-bom.csv schematic plot, bill of materials (72 parts; then H1/H2, board-only holes, no part, and the hardware lines HW1-HW6)
memory-v1.3-eagle.kicad_sym, .pretty/, sym-lib-table, fp-lib-table the built card's converted libraries, copied (same nickname memory-v1.3-eagle; was memory-v1.3-fusion-export-2026-09-24-eagle before the rename, see below)
options-top-edge-J2/ the top-edge record: memory-v2.0.kicad_pcb (the board finished from option B, + .kicad_pro / .kicad_dru) and its fab outputs (memory-v2.0-gerbers.zip, gerbers/, memory-v2.0-jlcpcb-order.txt, memory-v2.0-render-{top,bottom}.png, memory-v2.0-placement.pdf); the three re-layout placements memory-v2.0-relayout-{a,b,c}.kicad_pcb / .kicad_pro / .kicad_dru, their trial routes -trial.* and images -render-top.png, -placement.png, -trial.png; reports/ (memory-v2.0-final.txt, -drc.json / -drc.rpt, -make.txt, -placement-check.txt, per option relayout-X-*)
placements.py, space_check.py, options-keep-copper/ the blocked keep-the-built-copper options (record, above)
reports/ the v2.0 board's memory-v2.0-make.txt, -order.txt, -placement-check.txt, -drc.json / -drc.rpt, -final.txt, -fab.txt; ERC (.rpt, .json, erc-summary.txt), netlist (.net), netlist-proof.txt (the standoff options' reports are in options-standoff/reports/)

Rebuild

hardware/cards/memory/kicad/v2.0/build.sh                     # verify the committed v2.0 board and REGENERATE its
                                                              # fab outputs (gerbers + zip, drill, renders,
                                                              # placement PDF, order note, 1:1 PDF, BOM); verify
                                                              # the committed standoff options + trial routes,
                                                              # remake their images and 1:1 PDFs, re-check the
                                                              # top-edge record (~10 min; no routing)
FINAL=trial hardware/cards/memory/kicad/v2.0/build.sh         # remake memory-v2.0.kicad_pcb from standoff E's
                                                              # committed trial route (72 vias) - stops at add_wp
                                                              # (JP3 and R15 are drawn for the route of order 15)
FINAL=route SEEDS=15 hardware/cards/memory/kicad/v2.0/build.sh    # route standoff E again in component order 15
                                                              # (the committed board's route) and remake the board
                                                              # (make-e, then add_wp: JP3, add_pd: R15);
                                                              # other SEEDS: those orders, the best kept
STANDOFF="c d e" hardware/cards/memory/kicad/v2.0/build.sh    # regenerate those standoff boards and route each
                                                              # anew (one Freerouting run per DSN component order
                                                              # in SEEDS, default "0 1 2 3 4 5 6 7", in parallel;
                                                              # the best kept; ~6 min per option)
STANDOFF="a" NOROUTE=1 hardware/cards/memory/kicad/v2.0/build.sh   # regenerate a board, keep its committed trial
OPTS="e" hardware/cards/memory/kicad/v2.0/build.sh            # only these standoff options
FROM=trial hardware/cards/memory/kicad/v2.0/build.sh          # top-edge record: remake its finished board (and fab
                                                              # outputs) from option B's committed trial route
ROUTE=1 ROUTES=4 hardware/cards/memory/kicad/v2.0/build.sh    # top-edge record: route option B anew
RELAYOUT="a b c" hardware/cards/memory/kicad/v2.0/build.sh    # top-edge record: regenerate the three option boards
                                                              # + new trial routes (NOROUTE=1: keep the trials)
KEEPCOPPER="a b c" hardware/cards/memory/kicad/v2.0/build.sh  # also regenerate the keep-copper record

A plain run: schematic + ERC; the v2.0 board's placement check, DRC with schematic parity, finish_v2.py verify, fab outputs (fab-e, drill-check) and 1:1 print; per standoff option the placement check, DRC with schematic parity, airwire, the trial route's numbers and DRC, render, placement and trial plots, the 1:1 PDF; the top-edge finished board's placement check, DRC and finish_v2.py verify; the netlist proof over every committed board; schematic PDF and BOM (+ bom-hw). Freerouting is not deterministic under load (and slow on a loaded machine), so the committed boards are the master; a new route replaces one only when committed. The gerbers and drill files carry their creation time, so each plain run rewrites them (no other change). It reads ../v1.3 (through a scratch copy) and ../../../cf/kicad/v1.0/cf_netlist.py + gen_cf.py (read-only); Freerouting from ~/freerouting/freerouting.jar (FRJAR=), watchdog WATCHDOG= s.

Results (build of 2026-09-30: the v2.0 board with JP3 and R15 + the standoff options A-E)

  • The v2.0 board (standoff E + JP3 + R15): PASS - 0 unrouted, 72 through vias, 12,808 mm, DRC 0 copper violations / 0 unconnected, planes one piece each, silkscreen clean, H1 / H2 in the NPTH drill file, placement check OK, netlist proof MATCH (reports/memory-v2.0-final.txt, -placement-check.txt, -fab.txt). Not ordered.
  • Netlist proof: MATCH. v2.0 schematic = the built v1.3 (53 parts, 169 nets, IC15 included) minus C20-C23 (each checked to be pin 1 GND / pin 2 VCC and nothing else on v1.3) + CF section (21 parts, 27 own nets, 69 pins on 17 shared nets) + JP3 (rule 7: the v1.3 net of IC13.27 checked to be exactly IC1.27, IC2.27, IC6.4, IC13.27 before the pin moves) + R15 (rule 8: the net ADDR15 checked to be exactly IC10.4, IC9.17, X1.A18 before R15 joins it): 72 parts, 187 nets, 692 pins, 33 unconnected pins (10 v1.3 + 23 documented CF no-connects). The v2.0 board equals the schematic pad for pad plus the two board-only standoff holes H1/H2, and must carry JP3 and R15; the five standoff boards and their trial routes (made before JP3 and R15) equal the schematic without rules 7 and 8, plus H1/H2; the top-edge finished board equals the schematic without rules 7 and 8; the three top-edge re-layout boards, their trial routes and the three keep-copper boards (records made before the removal) equal the schematic without rules 7 and 8 plus exactly C20-C23 as on v1.3 (reports/netlist-proof.txt).
  • ERC: PASS (99 vs the built card's 104, all explained: reports/erc-summary.txt).
  • Standoff placements: OK for A-E (options-standoff/reports/standoff-X-placement-check.txt): no overlaps, pads 0.5 mm inside the edge, X1 / JP1 / U$1 group as built, J2 oriented for a straight ribbon, nothing tall under the adapter or the ribbon, the standoff holes clear (A / B: nearest pad 4.9 mm, body 4.6 mm; C-E: pad 4.2 mm, body 3.5 mm from a hole centre), the ROM keep-clear zone empty and away from the adapter (A / B 44.8 mm, C 4.6, D 5.8, E 5.1 mm); C-E: J2's plug envelope clear (A / B: NOTE, made before that rule); schematic parity: nothing new (beyond the two items of a board made before JP3 and R15: JP3 missing, IC13 pad 27 on -WE, R15 missing).
  • Standoff trial routes: complete for A (94 vias, 13,540 mm), B (100 vias, 13,748 mm), C (82 vias, 14,096 mm), D (77 vias, 12,502 mm) and E (72 vias, 12,579 mm), 0 DRC copper violations.
  • Top-edge record (option B finished board): PASS as before - 0 unrouted, 43 through vias, 11,779 mm, DRC 0 copper violations, planes one piece each, silkscreen clean (options-top-edge-J2/reports/memory-v2.0-final.txt).
  • Not ordered: E was chosen (2026-09-25), finished as the v2.0 board; open before ordering: the ribbon plug's pin 20 (the power-pad order: resolved 2026-09-26).

Last updated 26 October 2026