# JLCPCB order files — kicad_led_ring_offset

## 2026-11-13 — connector corner moved for the heat plate; CP1 surface-mount

- **Why:** the enclosure's aluminium heat plate under the ring needs a window wherever through-hole pins come out of the back. `J1`'s pins
  ran to within 2.5 mm of the bottom edge and 5.9 mm of `MH1`, so the window had to be an open notch with only 1.07 mm of clearance
  on one side.
- **`J1`** moved 4 mm up and 1 mm left (pins on x = 235, pin 1 at y = 233.25); **`J2`, `R1`, `R2`** moved 4 mm up with it, and their tracks
  and vias followed (the `NTC_RING` track's last bend too). The silkscreen pin labels by `J2` now read `DAT GND CLK GND NTC`, between `J2` and `J1`.
- **`CP1`:** the radial CX 1000 uF (C439782, through-hole) -> **ROQANG RVT1C102M1010, 1000 uF 16 V SMD, D10 x L10.2, C72470** on KiCad's
  `CP_Elec_10x10`, at (219, 225.4); its ground pad has three vias to the bottom ground pour. LCSC stock 10,810 on 2026-11-13; the JLCPCB
  tier was not checked.
- **`J2`** stays through-hole: neither a top-entry nor a 5-pin side-entry surface-mount JST XH is stocked at LCSC, and KiCad has no
  footprint for one.
- **Part counts:** 360 SMD and 2 THT (`J1`, `J2`); component cost $18.07 SMD-only and $18.40 full (`assembly_cost_compare.csv`), about $15.58 a
  board at 1 board by the LCSC price ladder (`ring_bom_cost.csv`).
- **CPL:** `tools/check_cpl_rotation.py` now runs (with `easyeda2kicad` installed; pass that interpreter's full path) and decided every part:
  `CP1` +0 (pads matched by number, so the polarity is right), `J1` +0, `J2` +180, the LEDs +180. It now keeps the last run's turn for any part
  EasyEDA doesn't return (it throttles), and writes nothing when it fetched nothing.
- **LED map:** `tools/gen_led_map.py` read the chain from the old SK6812 pins (2 and 4); it now uses the SK9822-A's SDI (1) and SDO (6), and
  `src/led_map.h` comes out unchanged, so no LED moved.
- ERC 0; DRC with schematic parity 0 violations, 0 unconnected, 0 parity issues. Gerbers, drill, BOM/CPL, PDFs and reports regenerated.
  Not tested on hardware.

## 2026-11-10 — JST VH power connector, 5-pin signal connector, ring thermistor TH1

- **`J1`:** Molex Mini-Fit Jr 2x3 right-angle (C114098) -> **JST VH 4-pin side entry B4PS-VH(LF)(SN), C157996**: 1-2 +5V, 3-4 GND, pin-for-pin with the mainboard's `J5` (B4P-VH) through a VHR-4N cable (SVH-41T-P1.1 crimps, 16-18 AWG). It sits in the bottom-right corner, pins on a vertical line at x = 236 (pin 1 at the top), with its opening toward the left (the old part's +x direction would have put the plug against `MH1`); `CP1` moved up 0.6 mm to clear it. Both pours reach the pads as before.
- **`J2`:** JST XH 4-pin -> **5-pin B5B-XH-A(LF)(SN), C157991** (pins 1-4 where they were; 5 = `NTC_RING`).
- **`TH1`:** Murata NCP18XH103F03RB (10k 1 %, B25/85 3434 K, 0603), **C13564**, on the top side at (150, 133), just above the centre hole among the inner LEDs, between `NTC_RING` and GND (its own GND via beside the pad). `NTC_RING` runs as one 0.2 mm track (F.Cu out of `TH1`, then B.Cu) to `J2` pin 5. The mainboard has the 10k pull-up.
- **Part counts:** 359 SMD parts and 3 THT parts (`CP1`, `J1`, `J2`); component cost about $17.97 SMD-only and $18.38 full (JLCPCB prices of 2026-11-09/10).
- **CPL:** `TH1` +0 (as `R1`); `J1`'s offset is not known (no EasyEDA footprint for C157996 on the day): it keeps KiCad's rotation, so check it in the preview. The LEDs' +180 is unchanged.
- ERC 0; DRC with schematic parity 0 violations, 0 unconnected, 0 parity issues. Gerbers, drill, BOM/CPL, PDFs and reports regenerated. Not tested on hardware.

## 2026-11-09 — LEDs are now the SK9822-A (data + clock); new signal connector J2

- **`D1`-`D178` are OPSCO SK9822-A-000, LCSC C5378730** (APA102-type: data and clock; 27 kHz PWM, so the ring films without flicker). 18,675 at JLCPCB and 15,780 at LCSC retail on 2026-11-09, enough for about 100 rings from one maker; $0.09 each at 100+.
- **Footprint:** project library `LEDRing.pretty` (`fp-lib-table`), `LED_SK9822-A_5.0x5.0mm_P1.6mm`, from the maker's land pattern (1.8 x 1.2 mm pads, 1.6 mm pitch, 3.4 mm between the columns). Symbol: KiCad's stock `LED:APA102` (same pin numbers: 1 SDI, 2 CKI, 3 GND, 4 VDD, 5 CKO, 6 SDO). `tools/check_cpl_rotation.py` matched JLCPCB's own SK9822-A footprint pad for pad (worst 0.15 mm): every LED again needs +180 in the CPL.
- **Same positions** for every LED and capacitor. With inputs on one side and outputs on the other, each hop in a row is two straight F.Cu traces (data at the top pads, clock at the middle ones). Each LED's ground pad goes straight down to one via. The 17 row-to-row links (and the jump under the centre hole) are two B.Cu traces between vias beside the pads.
- **Input:** `J2`, a JST XH 4-pin header (B4B-XH-A, C144395; 1 DATA, 2 GND, 3 CLK, 4 GND) carries data and clock in their own cable; `R1` (data) and the new `R2` (clock), both 470R, sit at the input as the datasheet requires. The pair runs on B.Cu up the right edge and along the top to `D1`, where the data line used to run. **`J1` (Mini-Fit) is power only:** its pins 1 and 2 are unconnected.
- **Electrical limits (datasheet):** VDD 5.3 V maximum, so keep the 5 V supply at 5.1 V. 18 mA per colour at the full 5-bit current (31): unlimited full white would be about 9.6 A, over the RD-85A's 8 A, so the firmware's current limit is required. The maker recommends at most 22 (12.2 mA per colour, about 6.5 A full white). Colour order RBG.
- ERC 0; DRC with schematic parity 0 violations, 0 unconnected, 0 parity issues. Gerbers, drill, BOM/CPL, PDFs, reports and the cost files regenerated. Not tested on hardware.

## 2026-11-08 — LED is now the SKC6812RV; CPL rotation fixed for the LEDs

- **`D1`-`D178` are OPSCO SKC6812RV-000, LCSC C2890040** (83,968 in stock, $0.059 at 150+, on 2026-11-08), instead of the SK6812-012 (C5378720, 22,963 in stock). Reason: 4 kHz PWM instead of 1 kHz, so the ring films with a quarter of the flicker. Checked against both maker datasheets: same pinout (1 GND, 2 DIN, 3 VDD, 4 DOUT, same corner arrangement), same 12 mA per colour and brightness, GRB at 800 kbit/s, same timing (T0H 0.25-0.40 us, T1H 0.65-1.00 us, reset over 200 us). The body is 5.0 x 5.0 mm instead of 5.4 x 5.0; its recommended pads (1.5 x 1.1 mm) sit 0.1 mm inside the board's pads, so the footprint is unchanged. JLCPCB's footprints for the two parts have the same pad numbering.
- **CPL rotation fixed.** JLCPCB's (EasyEDA) footprint for both LEDs has pad 1 at the bottom right, KiCad's at the top left, so KiCad's rotation alone would have placed every LED turned 180 degrees, with GND on the +5 V pad. `tools/check_cpl_rotation.py` (a copy of the mainboard's) now writes `cpl_rotation_offsets.json` (+180 for every LED, 0 for the capacitors, `R1` and `CP1`; `J1` undecided, it is placed by hand from the silkscreen) and `tools/build_jlc_assembly.py` adds it to the CPL. Still look at the LEDs in JLCPCB's placement preview.
- Not checked: whether the SKC6812RV is also "standard PCBA only" (the SK6812 was). JLCPCB shows it at upload.
- **Current figures corrected:** both LEDs' datasheets give 12 mA per colour (13.5 mA maximum for the SKC6812RV), so full white is about 6.5 A (7.3 A maximum), not the 10.7 A (60 mA per LED) this folder's older notes and the 2026-09-14 voltage-drop study assumed; that study's figures are therefore pessimistic. WLED is set to 36 mA per LED and 4600 mA, about 4.5 A of ring current.

## 2026-11-08 — every part on the top side (single-sided assembly)

- **The 178 decoupling capacitors moved from B.Cu to F.Cu**, each 4.1 mm below its LED (LED-local coordinates), beside the LED's +5 V pad, with its +5 V pad in the F.Cu pour and its GND pad on a 0.3 mm stub to one 0.6/0.3 mm via into the B.Cu ground plane. The 178 +5 V stitch vias and B.Cu stubs that fed the old bottom-side capacitors are gone, so the via count is unchanged (388). Smallest courtyard gap between a capacitor and its LED: 0.58 mm (JLCPCB's placement check needs about 0.5 mm).
- **Why:** with every part on one side JLCPCB charges single-sided setup and stencil, not double-sided: $33.77 less per order on the Standard tier (setup $51.12 to $25.56, stencil $16.42 to $8.21). The SK6812 still keeps the board on the Standard tier.
- The 2026-09 section below about capacitors directly under their LEDs (and the 0.5 mm shift for JLCPCB's spacing check) is history; B.Paste is now empty.
- DRC with schematic parity: 0 violations, 0 unconnected, 0 footprint errors (silkscreen included); ERC 0. BOM/CPL (all 359 placements on layer T), gerbers, `LEDRing_pcb.pdf` and the reports regenerated.

## 2026-10-11 — documentation folded into the main project; reports refreshed

- No board or part changes: BOM, CPL and gerbers are unchanged. `erc_report.rpt` and `drc_report.rpt` were regenerated (ERC 0; DRC with schematic parity 0 violations, 0 unconnected, 0 parity issues); the old DRC report still listed the `D89` jumper as unconnected.
- The ring is now described in the project's Hardware Overview (section 6) and README, including this folder's ordering notes.

## 2026-09-29 — D89->D90 routed, schematic parity cleaned up

- **`LED_D89_DOUT` routed around the centre hole** on B.Cu (details below), replacing the
  hand-soldered jumper wire. `JMP89A`/`JMP89B` removed.
- **Parity cleanup:** the PCB's net names now carry the schematic's `/` prefix (179 nets), and
  every footprint has its full library ID (`LED_SMD:...`, etc.). The four mounting holes are
  marked board-only. A pad-by-pad comparison showed all 359 footprints' copper is identical to the
  KiCad 10 library, so the project now ignores `lib_footprint_mismatch` (differences are
  silkscreen/text only). DRC with schematic parity: **0 violations, 0 unconnected, 0 footprint
  errors** (was 1 unconnected + 404 parity notes). ERC: clean.
- `tools/build_jlc_assembly.py` now picks the newest installed `kicad-cli` (it picked KiCad 9,
  which can't read a KiCad 10 board). BOM/CPL regenerated: **unchanged**. Gerbers re-exported.

Generated 2026-08-26 from `LEDRing.kicad_pcb` / `LEDRing.kicad_sch` (commit 79b02df).

## 2026-09-20 — gerbers were stale since the J1 connector swap; regenerated

Found during a fresh pre-order review: `LEDRing_gerbers.zip` was last regenerated in the commit
that first brought this board into the repo (2026-08-26), but `J1` was swapped from a Phoenix
screw terminal to the Molex Mini-Fit Jr 5569-06A2 in commit `083dfb4` (2026-08-28) and the
gerbers were never re-exported afterward — the committed zip still had the *old* connector's hole
size (1.3mm) and pad geometry, not the Mini-Fit Jr's (1.8mm). `BOM`/`CPL`/`assembly_cost_compare.csv`
were already correct (`FP_MAP` in `tools/build_jlc_assembly.py` already had the Mini-Fit Jr
entry, confirmed by re-running the script — byte-identical output) — only the gerbers/drill
lagged. Re-exported via `kicad-cli pcb export gerbers`/`export drill` from the current
`LEDRing.kicad_pcb`; new drill tool table confirms the fix (`T3C1.800` where it used to read
`T3C1.300`). Also fixed `tools/build_jlc_assembly.py`'s hardcoded KiCad 9.0 `Program Files` path
(didn't exist in the environment that caught this) to search `PATH` + common install locations
instead, matching the mainboard's copy of the same script — the stale gerbers likely went
unnoticed specifically because the script couldn't be easily re-run to catch drift like this.

## 2026-09-10 — full assembly, 0 sourcing-risk (SMD-only vs full breakout)

BOM/CPL are now broken out SMD-only vs full assembly (see `ASSEMBLY_COMPARE.md`).
The board's only two THT parts both substitute to in-stock JLCPCB wave-solder
parts whose footprints already match — so **full assembly needs zero hand-soldering
and no board changes**: `CP1` 1000µF radial → **C439782** (D10/5mm-pitch), and
`J1` Molex 5569-06A2 right-angle → **C114098** (mates the mainboard `J5` harness).
Generated by `tools/build_jlc_assembly.py` (re-run after any board change).

## Files

- `LEDRing_gerbers.zip` — Gerbers (F/B Cu, Paste, SilkS, Mask, Edge.Cuts) + Excellon drill
  (PTH/NPTH separate), re-exported 2026-09-20 from the current board (see above). Upload directly
  to JLCPCB's "Add Gerber file" step. Since 2026-11-09 the ring is ordered at **1oz copper**
  (JLCPCB's default); a 7.5 A fuse in the 5 V harness caps a fault (Hardware Overview, section 6).
- `LEDRing_CPL_SMD.csv` (357 rows) / `LEDRing_CPL_FULL.csv` (359, adds CP1+J1) — pick-and-place,
  already in JLCPCB's format (`Designator,Mid X,Mid Y,Layer,Rotation`, `mm`-suffixed coords, `T`/`B`).
- `LEDRing_BOM_SMD.csv` / `LEDRing_BOM_FULL.csv` — consolidated one row per unique part; the FULL
  file adds `Assembly`/`Source status`/`Note` columns (drop them if JLCPCB's parser is strict).
- `assembly_cost_compare.csv` — per-part **component** cost at this board's real per-board
  quantity (LCSC unit price × qty, at the price-break tier that quantity actually reaches),
  plus SMD-only vs full-assembly totals. Pricing pulled from each part's live LCSC page on
  2026-09-12 and will drift — this is component cost only, **not** JLCPCB's separate,
  order-quantity-dependent PCBA assembly/setup fee. Regenerate via
  `tools/build_jlc_assembly.py` (see its `PRICE_MAP` to refresh prices).

  *(The old single-variant `LEDRing_BOM.csv/.xlsx` + `LEDRing_CPL.csv/.xlsx` were removed. `.xlsx`
  variants are no longer produced; JLCPCB accepts the `.csv` directly.)*

## Assembly scope

Full assembly is now viable (all 359 parts are JLCPCB-assemblable). For the cheapest option,
`*_SMD.csv` still covers only the SMD parts (LEDs, caps, R1); the two THT parts (`CP1`, `J1`) are
then hand-soldered. `MH1–MH4` are mounting holes (nothing to assemble). See `ASSEMBLY_COMPARE.md`.

## LCSC part numbers

| Part | LCSC # | Status | Notes |
|---|---|---|---|
| SK6812 5050 LED | C5378720 | Extended | OPSCO Optoelectronics, "SK6812-012". Original pick (C9900035077, JLCPCB's own "5050LED" listing) went out of stock. **Pinout verified directly against the real manufacturer datasheet**: pin1=GND, pin2=DIN, pin3=VDD, pin4=DOUT — matches this board's footprint exactly. A different candidate, "SK6812-B" (C5380881), was checked and rejected: its datasheet shows pin1=VDD, pin3=GND — reversed — which would put +5V and GND backwards on every LED. If this part ever goes out of stock again, re-verify pinout the same way before substituting anything with "SK6812" in the name; the family isn't pin-consistent across variants. |
| 100nF 0603 X7R cap | C14663 | Basic | Yageo CC0603KRX7R9BB104, 50V, ±10%. |
| 470R 0603 resistor | C23179 | — | Uniroyal 0603WAF4700T5E, 1% |

JLCPCB's BOM upload tool will re-validate these against their live catalog (stock levels change
often) — still worth a last check there before ordering, but the pinout risk specifically has
been confirmed from source datasheets, not just catalog listings.

## Fixed: capacitors weren't importing at all (real root cause)

Not a part-number problem, even though two different verified 0603/100nF/Basic candidates
(C14663, then C1590) both failed to import while the LED and R1 rows from the exact same files
worked every time. The actual cause: on this board, every decoupling cap sits **directly
underneath its LED** (same X,Y centroid, 0.0mm apart — cap on B.Cu, LED on F.Cu, opposite faces,
completely valid physically). JLCPCB's placement-matching tool checks minimum spacing between
*any* two designators in the flat XY plane without apparently accounting for layer, and silently
drops components that violate it rather than erroring — so all 178 caps were being rejected as a
group for sitting exactly on top of their LEDs, while LEDs themselves (unique positions) sailed
through.

**Fixed on the PCB itself** (not just in these export files): shifted all 178 cap footprints
0.5mm sideways relative to their LED (still effectively right underneath for decoupling
purposes — 0.5mm is nothing at this scale), and re-anchored each cap's +5V stitching trace to
follow. Verified 0 DRC violations (reproduced twice) after the change, and confirmed the new
minimum spacing between any two components is a clean 0.5mm everywhere. All files above were
regenerated from the updated board.

## D89 -> D90 data link: now a routed trace (2026-09-29)

`LED_D89_DOUT` used to be left open on the PCB (D89 and D90 sit either side of the 25.4mm centre
hole), to be closed after assembly with a hand-soldered wire between two vias. It is now routed:
a 0.2mm B.Cu trace from the D89-side via (129.01, 147.12) around the top of the hole to the
D90-side via (170.99, 152.88), following a polygon about 14.2mm from the hole centre. Every chord
stays at least 13.7mm from the centre (hole radius 12.7mm + 0.5mm copper-edge clearance + half the
track). The two dead-end stubs and the PCB-only `JMP89A`/`JMP89B` wire pads are gone. The same
detour already carried `LED_D76_DOUT` around the hole on F.Cu. **No manual step remains:** the
whole data chain is copper, and DRC reports 0 violations and **0 unconnected** (it used to report
the one intentional open).

## Known open items before ordering (see also project memory)

- **Copper weight**: not specified in the board file. **1oz** (JLCPCB's default) since 2026-11-09: about
  8mV of drop at 4.5A, and the 7.5 A fuse in the 5 V harness caps a fault. (It was 2oz before; the IR-drop
  figures below are from then and double at 1oz.)
- **IR-drop checked (2026-09-14): negligible.** No SPICE/FEM field solver was available, so
  this was done as a DC resistor-mesh estimate instead: the real `+5V` (F.Cu) and `GND` (B.Cu)
  filled-zone polygons were pulled straight from `LEDRing.kicad_pcb` via `pcbnew`, rasterized to
  a 1mm grid, and solved as a conjugate-gradient resistor network (one grid square = the sheet
  resistance, independent of grid pitch) with 10.7A injected/returned at `J1` and 60.1mA sunk/
  sourced at each of the 178 LEDs at its real position. Worst case (farthest LEDs from `J1`,
  `D1`/`D14`/`D15`) is **~9.6mV at 20°C, ~11.6mV at a hot 70°C plane** (2oz copper) — under 0.25%
  of 5V, nowhere near SK6812's operating margin. The full F.Cu/B.Cu plane split (not narrow
  traces) is why: current spreads across nearly the whole board instead of funneling through a
  choke point. Caveat: this is a steady-state DC estimate (real via/pad contact resistance and
  switching-transient droop aren't modeled), not a substitute for a bench measurement at the
  farthest LED under real full-white load, but it rules out DC IR-drop as a design risk.
- ~~D89's DOUT jumper wire~~ — no longer needed; the link is routed on the PCB (see above).
