Esp32node wip

Illuminate 7 Mk2 — crossover board

One passive crossover board per speaker, so build two. Single-sided, through-hole only, CNC isolation-milled with an 0.8 mm end mill (the DTU 62768 process). The topology is the PrintYourSpeakers reference crossover, unchanged; only the component values are substituted for what the DTU component shop actually stocks.

Status: schematic done (ERC 0 violations), board routed by hand on B.Cu, 144.5 × 110 mm, four M4 corner holes, DRC clean. Mill and laser files are in production/illuminate7mk2-crossover/ (Gerbers + Excellon for the CAM, _silk_top.dxf for the laser silkscreen). Coils: L102 may be a shop 270 µH if it passes the LCR check; L101, L201 and L202 are to be wound.

Circuit

IN+ ─┬─[ C 2u2 ∥ L 0.20mH ∥ R 9R4 ]─ A ─[ C 5u5 ]─ B ─[ C 10u1 ]─ TWEETER +
     │                                             └─[ L 0.25mH ]─┐
     │                                                            │
     └─[ C 41u ∥ L 0.70mH ∥ R 20R ]─ C ─[ L 2.0mH ]─ D ───────────┼─ WOOFER +
                                                    └─[ C 11u5 ]──┤
IN− ─────────────────────────────────────────────────────────────┴─ both −

The GND symbol on the sheet is IN−, the amplifier's negative speaker terminal and the common return for both drivers. It is not chassis earth, and the left and right boards' returns must stay separate — the Fosi V3 is a bridged (BTL) class-D amp and its negative outputs are not ground.

BOM

From the DTU component shop — per board

For two boards: double every quantity — 4 × 2u2, 6 × 3u3, 2 × 6u8, 12 × 8u2, 4 × 4R7 5W, 4 × 10R 5W, 6 × 2-pole screw terminals.

How the parallel groups add up:

Coils — buy these, the shop has nothing usable

The shop stocks only small ferrite chokes with no current rating and a few bare toroid cores, and no magnet wire. All four coils are air-core, 0.8 mm (20 AWG) wire. Per board:

Buy eight coils in total, two of each. Air-core only: an iron or ferrite core saturates and distorts at woofer levels. Check the DCR on the datasheet — it is part of the design, not a parasitic, and a coil with materially lower DCR shifts the level of that branch.

Or wind them yourself

Air-core coils are just wire on a bobbin, so with enamelled copper wire and an LCR meter they can be wound at home. Use 0.8 mm wire: it is what the Dayton parts use, and it lands the DCR on the design value. Starting points (Wheeler multilayer formula, 3D-printed bobbin, hand-wound with ~15 % slack):

Total wire for two boards: about 140 m of 0.8 mm. Procedure:

1. Print a bobbin with the core diameter above, flanges 2 mm taller than the expected winding depth, and a slot in one flange for the start lead.
2. Wind about 5 % fewer turns than the table, tight and in even layers, keeping the wire under tension. Count turns.
3. Measure L on the LCR meter at 1 kHz. Inductance goes with turns squared, so add turns as N_new = N × sqrt(L_target / L_measured). Aim for ±3 %.
4. Measure DCR on the meter's DC-resistance range (or 4-wire if it has it) and compare with the target above. If the coil comes out lower than target, add a shop 5 W resistor in series to make up the difference (0.1–0.68 Ω are stocked); if it is more than ~0.1 Ω higher, the wire is thinner than 0.8 mm or the coil is looser than assumed, and it is better to rewind.
5. Fix the winding with a few wraps of tape or a drop of glue, and keep the two coils of each branch at least one coil diameter apart, or at right angles, on the board so they do not couple.

Thicker wire (1.0 mm) gives about 30 % lower DCR than the design, so it needs the series-resistor trim in step 4 on every coil; thinner wire (0.6 mm) makes the DCR too high and should not be used for L202.

Capacitor voltage ratings (read off the parts)

The Fosi V3 runs from 48 V and is bridged, so the input can swing about ±45 V. The shop parts, as printed on them:

Does this make an adequate crossover?

Yes. sim/crossover_ac.cir runs both versions side by side in ngspice with the drivers modelled as plain resistors (4 Ω tweeter, 8 Ω woofer) and the coil DCRs included, and sim/compare.py reports the difference over 100 Hz – 20 kHz:

Nowhere in the band does either branch move more than 0.54 dB, and the woofer stays under 0.5 dB everywhere. That is below the tolerance of the drivers themselves (Dayton quotes ±10 % on Thiele-Small parameters, and 5 % film caps are already worth a few tenths of a dB), and well under what is audible on a broad, smooth deviation like this. The substituted set is fine.

Reproduce it with:

cd sim && ngspice -b crossover_ac.cir && python3 compare.py

Board layout

tools/pcb_build.py builds the .kicad_pcb from the schematic netlist and places it on a fixed floorplan that follows the signal flow, packed from the footprints' real courtyards. 151 × 120 mm on the measured footprints, inside the mill's 203 × 152 mm envelope. Re-run after any footprint change:

kicad-cli sch export netlist --format kicadsexpr -o /tmp/xo.net illuminate7mk2-crossover.kicad_sch
python3 ~/.claude/skills/kicad-laser-pcb/scripts/pcb_netlist_json.py /tmp/xo.net /tmp/xo.json
python3 tools/pcb_build.py /tmp/xo.json illuminate7mk2-crossover.kicad_pcb

 row A   L101 pads | C101 R101 R102 | C102 C103 | L102 pads | C104 C105 | J2 TWEETER   (top)
 row C   J1 IN, R201 R202 | C201 C202 C203 C204 C205 | L201 pads                     (middle)
 row B   L202 pads | C206 C207 | J3 WOOFER                                           (bottom)

• The coils are not on the board. They would not fit the mill envelope, so each coil has only its two lead pads (crossover:L_OffBoard_P10.16mm, 10.16 mm pitch, 1.4 mm holes) at a board edge: L101 left edge top, L202 left edge bottom, L201 right edge middle, L102 top row between the tweeter caps. Mount the coil bodies overhanging the edge next to their pads, or glue them to the enclosure beside the board, and bring the leads to the pads. Keep any two coils at least one coil diameter apart, and never stack one on another.
• Input on the left edge, tweeter out top-right, woofer out bottom-right.
• Copper is B.Cu only, single-sided. A GND zone is defined on B.Cu (the return for both drivers) but not filled — fill it after routing.
• Design rules: 0.85 mm clearance, 1.0 mm minimum track, 2.0 mm default track. Use 2 mm or wider for everything; this board carries amps.
• Four M4 holes in the corners, 6 mm in. The Illuminate enclosure has five M4 inserts for its own crossover plate; match those positions once you have the printed part, by editing HOLE_INSET / the hole list in the build script.
• The terminal-block footprints show a small triangle on the wire-entry side. J1 faces left, J2/J3 face right; if the real blocks turn out to open the other way, flip the rotation (90 ↔ 270) in ROW_A/B/C.
• DRC: 0 violations. Placement score: rotation, spacing and alignment pass; cohesion is 0.43 against a 0.25 threshold, which is the price of pushing the coil pads to the edges.

Routing notes for the hand pass: IN+ is the big net (11 pads, J1 → L101 tank, R101, C101, and the whole woofer tank). Run it as one wide bus along the left side and the middle row. GND has only six pads and the pour carries it. The circuit is series-parallel, so nothing forces a wire bridge: it routes on one layer with zero jumpers if the placement is respected.

Measured footprints

Every shop part was measured with calipers on 2026-09-24 (pitch = leads outside to outside minus one lead Ø). The same table is in the DTU-EKB footprint repo (DTU-EKB/KiCad-components), so these never need measuring again.

Still open: the coil lead spacing if the wire ends up thicker than 1.0 mm (raise DRILL in tools/make_coil_footprints.py), and the enclosure's M4 insert positions. pcb_build.py drops the bottom edge until the bottom corner holes clear every courtyard by 1 mm.

Notes on manufacturability

Every footprint currently on the board clears the 0.8 mm mill floor with room to spare — the smallest pad-to-pad gap is 2.2 mm on the screw terminals, so no .kicad_dru exceptions are needed. The netclass is already set to the CNC profile (1.0 mm track, 0.85 mm clearance).

The coil footprints live in a project library, registered in fp-lib-table as crossover. KiCad reads that at project load, so open the project rather than the bare .kicad_sch if a footprint shows up as missing.

To redraw the sheet after a change, edit tools/crossover_layout.py and run it — it rewrites both the .kicad_sch and the .kicad_pro, and verifies the netlist against the intended topology before it writes anything. Close KiCad first; it does not notice a .kicad_sch changing underneath it and will overwrite your file from its stale copy on save.