mangavalkandClaude Opus 5.5
dbc1f0041f
- Design docs: 12 V DC power supply, safety and bring-up, ESP32 interface, BOM - PSU schematic (schemdraw) and KiCad 10 carrier-board project with HV net classes - ESP32 PlatformIO firmware skeleton with HV watchdog toggle - Reference schematic of the Stern 520-5138-00 display PSU Co-Authored-By: Claude Opus 5.5 <noreply@anthropic.com>
KiCad project: PSU carrier board
Open plasma_dmd_psu.kicad_pro in KiCad 10.
The board carries the fuses, the HV watchdog, both regulators (copied from Stern 520-5138-00) and the connectors. The AliExpress modules sit off-board and connect through Phoenix 5.08 mm screw terminals:
| Connector | Goes to | Pins |
|---|---|---|
| J1 | 12 V DC brick | +12V, GND |
| J3 | Mini560 5 V buck | IN+, IN−, OUT+, OUT− |
| J4 | Relay module | VCC, GND, IN, COM, NO |
| J5 | NCH6100HV #1 (set 90 V) | VIN, GND, HV+ |
| J6 | Isolated DC-DC input | VIN, GND |
| J7 | NCH6100HV #2 (set 130 V) output | HV+ (→ GND), GND (→ −130 V raw) |
| J8 | ESP32 | 5V, GND, GPIO21 (watchdog) |
| J2 | Panel power, Molex KK-396 8-pin | Stern CN2 order: 1 −112V, 2 −100V, 3 key, 4–5 GND, 6 +5V, 7 +12V (via JP1), 8 +65V |
Wire the isolated DC-DC output straight to NCH6100HV #2's input, off-board. Both float at −130 V.
⚠️ J2 pinout is a placeholder. It follows the Stern supply, not necessarily your WPC panel. Map it to your panel before you plug anything in.
Files
| File | What |
|---|---|
gen_kicad.py |
Generates the schematic and the project's net classes from the PARTS table. The source of truth. |
check_netlist.py |
Exports the netlist with kicad-cli and checks every pin against PARTS |
plasma_dmd_psu.kicad_sch |
Generated schematic (labels-per-pin style: connectivity is by net label) |
plasma_dmd_psu.pdf |
Plot of the schematic |
python hardware/kicad/gen_kicad.py
python hardware/kicad/check_netlist.py
Re-running gen_kicad.py overwrites the schematic. Either keep editing PARTS and regenerate, or
stop using the generator once you start editing the schematic in KiCad.
Net classes (already in the project)
| Class | Nets | Clearance | Track |
|---|---|---|---|
| HV | +90V_RAW, +65V, −130V_RAW, −112V, −100V, HVP/HVN_MOD and all regulator internals | 3.0 mm | 0.6 mm |
| Power | GND, +12V*, +5V, +12V_PANEL | 0.3 mm | 1.0 mm |
| Default | Watchdog signals | 0.25 mm | 0.4 mm |
Making the PCB
- Open the PCB editor and choose Tools → Update PCB from Schematic (F8). All footprints arrive with ratsnest.
- Draw the board outline on
Edge.Cuts. - Placement tips:
- Keep the HV area (J5/J7, F4/F5, regulator, J2) on one side and the 12 V/5 V/watchdog on the other.
- Leave room for TO-220 heatsinks on Q3, Q5 and Q6. R13 (5 W) runs warm.
- Consider routed slots between the HV and low-voltage areas.
- Run DRC. The HV class enforces 3 mm to everything.
Verified so far
- The schematic loads in KiCad 10.0.6, and ERC reports 0 violations.
check_netlist.py: all 122 pins sit on the intended nets (31 nets).- All symbols and footprints come from the KiCad 10 standard libraries.
- Transistor pinouts match the footprints: MJE15030/31 are B-C-E (TO-220); MPSA42/92 are E-B-C (TO-92); 2N7000 is S-G-D.
Not verified: the circuit itself on real hardware, and the module current ratings.