hardware(pcb): USB-C power path burnout & smoke — soldering issue vs. structural flaw?

[engmung]

Area

pcb

What happened?

In Patternflow v3.0.0, a USB Type-C connector (USB1, 14-pin THT) was introduced as an alternative power input option (Path B) alongside the 2-pin screw terminal (Path A / J4).

Context behind choosing this specific USB-C part:

• The v3.0 board design deliberately avoided all SMD passives/components (100% Through-Hole / THT) to keep hand assembly accessible for DIY builders and to prevent potential cost surges if PCBA services were used later with SMT lines.
• To maintain this pure THT design goal, a 14-pin THT USB-C receptacle (SHOU HAN TYPE-C 14P CC-2.6 / LCSC C5187475) was selected. Note: Only power (VBUS/GND) and CC pins are used; data signals are not connected.

Observed Failure Behavior:

• Power source: 5V USB power bank.
• Assembly & multimeter checks: Hand-soldering the tight pin pitch of this 14P THT connector is extremely challenging. Pre-power multimeter checks were performed, but given the tight spacing, it remains ambiguous whether a subtle micro-bridge or high-resistance joint was missed.
• Delayed failure behavior: Upon powering on, the device works completely fine with no noticeable heat or issues for the first several tens of minutes (e.g., 20–30+ minutes).
• Sudden catastrophic burnout: After that initial normal operating window, smoke suddenly begins to emanate from a specific pin area. Once this occurs, it rapidly overheats and permanently fries the USB-C receptacle and surrounding power path.
• The exact pin location where the smoke/burnout initiates is highlighted in the photos below.

Key Questions for Community & Hardware Reviewers

1. Soldering Skill vs. Structural/Electrical Failure: Is this burnout genuinely a hand-soldering defect (e.g., micro solder bridges), or is it a structural/electrical failure inherent to this part or PCB layout when supplying the high peak current drawn by the 128x64 LED matrix?
2. Alternative Power-Only Connectors: If this 14-pin THT connector is structurally prone to burning out under load (or too difficult for hand assembly), what alternative power-only USB-C (e.g. 2-pin, 6-pin power-only THT/SMT) or power adapter connector parts would you recommend for future revisions and mass production/PCBA? (Note: Signal/data lines do NOT need to be connected — power-only).

Photos / Evidence

KiCad (Layout / Schematic)	Physical Board (Pin Location / Burned Result)
KiCad Layout (Zoomed Pin Area)	Marked Pin Location (Clean / Slightly Charred)
KiCad Power Section Schematic	Severely Burned Connector & Board

Potential Suspects to Investigate

1. Pin Current Rating & VBUS/GND Stress: High current draw of the LED matrix causing localized resistive heating on narrow THT pins/traces.
2. Internal Thermal Shorting / Footprint: Thermal expansion melting internal insulation or bridging adjacent pins under load.
3. Trace Layout & Thermal Relief: Insufficient copper weight/relief near the power pins.

Goal & Next Steps

• Determine whether the failure is assembly-related or a structural design flaw.
• Evaluate alternative power-only connector options for v3.1 / PCBA.
• Review PCB schematic & KiCad layout in hardware/pcb/ for necessary trace widening or protection additions.

[engmung]

Docs updated while this is investigated — the build guide now routes every build through the J4 screw terminal and marks USB1/R1/R2 as on hold (not withdrawn — the parts stay listed, flagged on-hold, since this input may well come back once the cause is settled).

The point emphasized everywhere is the one that makes this dangerous to shrug off: the failure is delayed. A clean pre-power multimeter check and 20–30 minutes of normal operation prove nothing, so "mine seems fine" isn't evidence the joint is safe.

Touched: BUILD_GUIDE §2/§5/§7/§9/§10, hardware/bom/bom_v3.0.csv + BOM README, and the v3.0.0 release notes. All of it points here. Every note says the docs get updated once the cause is determined.

[magsho]

• My thoughts what to do next:

1. Test existing PCB but with low load - disconnect led display completely or make it lowest brightness possible
2. Power it via USB-C and leave it for few hours, check the usb connector and pcb below it with hand, what's the temperature? Is it getting too hot with time?
3. Soldering - do you use any solder flux? It would help you with soldering such small components and make overall soldering more reliable.

• Why it fails? I think of two possibilities:

1. Tracks for 5V are too narrow - only 0,25 mm
   I measured current consumption by display and with the patterns I tested it's in the range of 0,5-1A on maximum brightness. I checked required track width for 0,5A and 0,25 mm is risky but it should work on short distance like you have assuming the pcb is 1 oz. If the pcb is 0.5 oz it will most likely overheat.

2. Bad soldering
   I look at this picture and I don't understand why the pins are not visible, are they too short for the thickness of pcb?

• PCB redesign
  I would redesign 5V track like below:
  -> blue tracks on both layers and width as large as possible
  -> yellow tracks can be one layer only and min. 1 mm width
  PCB has large ground planes on both layers - this is not necessary in this application, make ground plane only on bottom layer.
  I see the pads are not completely round which makes it harder to solder - make round pads for 5V pins.

[engmung]

@magsho
Thanks for the detailed feedback!

I’ll definitely try widening the 5V traces and run some tests with that layout. Not sure if I'll modify the GND plane or the footprint pads right away since it can be a bit tedious, but I'll incorporate what I can.

Honestly, hand-soldering USB-C itself is just inherently brutal, so USB-C is likely going to remain a PCBA-only option anyway.

Thanks again for taking the time to write this out!