SolarNodeChargeController

Solar Node Charge Controller

A small solar charger board for a single-cell (1S) Li-ion/LiPo battery, built for solar-powered LoRa mesh nodes such as SNAP v1.2. Up to four 5V panels feed a CN3791 MPPT buck charger. A switched output powers the node, and an INA219 reports voltage and current over I2C.

Designed in KiCad 10.

Status: the schematic is complete and passes ERC. The PCB (56.5 × 29 mm, 2mm corner chamfers, four M3 mounting holes, two layers) is placed and auto-routed with a clean DRC, but hasn't had a manual layout review. A first board has been wired up and tested with a XIAO + Wio-SX1262 on a custom Meshtastic build, and everything seems to work as expected so far, including the I2C sensor. A sunlight test in a real solar node is under way, with the expected voltage and charge current so far. See Testing.

Built for solar mesh nodes

This controller is meant for solar mesh nodes like the SNAP v1.2: Solar Node Adaptable Platform. It simplifies their build in three ways:

• Easy, clean connections: the panels, battery, node and switches each plug into their own connector.
• Improved solar charging: an MPPT charger tuned for 5V panels, with a diode for every panel built into the board.
• I2C power sensing: configurable for either the battery or the solar circuit.

I2C power sensors are supported natively by both Meshtastic and MeshCore. In most cases the node recognizes the INA219 automatically once it's connected.

In the SNAP v1.2 example build, shown below, the board replaces several separately wired parts:

Example wiring

Set SW3 to BATT to see the battery's charge and discharge current, or to SOLAR to see what the panels deliver.

The XIAO's I2C pins depend on the firmware build. D4 and D5 can't be used with the Wio-SX1262, because the radio uses them.

The INA219 uses address 0x40, which some other I2C sensors also use (for example the SHT21/HTU21D and HDC1080). If your node already has one of those, the two will clash.

In Meshtastic, enable power metrics in the telemetry settings so the readings are sent to the mesh.

Features

• Solar input: up to four 5V panels in parallel (Micro JST 1.25), each isolated by its own 1N5819WS Schottky (SOD-323) so a shaded or unplugged panel doesn't drag the others down.
• MPPT charging: CN3791 PWM buck charger with constant-voltage MPPT set to 4.58V input. Charges at 0.8A to 4.2V (CC/CV, trickle charge for deeply discharged cells, automatic recharge).
• Battery and load switching: connectors for two panel-mount switches. SW_BATT disconnects the battery from everything. SW_LOAD cuts only the output, so the battery keeps charging.
• Output: VOUT connector (Micro JST 1.25) that powers the module from the battery.
• Power monitoring: INA219 at I2C address 0x40. A slide switch selects whether it measures the solar input or the battery (bidirectional current plus voltage).
• Status LEDs: red while charging, green when charging is done.

Schematic

The schematic follows the CN3791 datasheet's typical application circuit (Figure 1), with these changes:

PCB

Every reference label sits next to its own part, clear of pads, other parts and the edge (DRC reports no silkscreen issues). The holes are plain non-plated 3.2mm M3 holes, 4mm in from each edge.

Silkscreen labels:

• Connector functions: vertical labels beside the right-hand connectors read SW_BATT (J7), SW_LOAD (J8), BATT (J5) and VOUT (J6).
• Solar inputs: one Solar_5V label, with a bracket along the four solar inputs (J1–J4).
• Polarity: - and + under the solar, battery and VOUT connectors (J1–J6), on the side of the matching pin.
• I2C connector: I2C under J9 on the front. The pin names (VCC, SDA, SCL, GND) are printed beside its pads on the back, since there's no room between the pads and the connectors on the front.
• SOLAR/BATT selector: solar/batt / i2c power sensor beside SW3 on the back, with "solar" at the end of the switch that has the PV pins and "batt" at the end with the battery pins.
• Back: the module ID, "Solar Charge Module v1.1 / by JaisorGadgets / Nov. 5, 2026".

Routing (by tools/route-pcb.py):

• Ground: the bottom layer is a solid GND plane. The top layer has a GND fill, and every surface-mount GND pad gets its own via down to the plane.
• Track widths: power paths are 0.8mm, necked to 0.4mm at small pads. Signals are 0.25mm.
• Kelvin sensing: the CN3791's current-sense pins and the INA219 selector's throws connect straight to the pads of their shunt resistors (R5, R6, R7).
• Layer use: about 80% of the copper length is on the top layer. The bottom-side tracks are short jumps, which keeps the ground plane mostly intact.
• Size: 208 track segments and 45 vias, 11 of which are GND stitching vias.
• Checks: DRC reports 0 violations and 0 unconnected items, and schematic parity is clean.

This is auto-routing, so review it before ordering, especially the buck converter's switching loop (C1 → Q1 → D2, which currently returns through the ground plane) and the few bottom-layer tracks that cut the plane.

Still to do: a manual layout review before ordering (see Fabrication).

Connectors

J1–J6 and J9 are Micro JST 1.25 (Molex PicoBlade-compatible) vertical headers, Molex 53047-0210 (2-pin) and 53047-0410 (4-pin). They mate with standard female cable housings (Molex 51021). J7 and J8 are standard 2.54mm vertical pin headers, which take a 2.54mm female housing or a jumper cap. Notes:

• Current: PicoBlade contacts are rated 1.0A. The charge current is set to 0.8A to stay under that on the battery connector (J5). Keep the module's load current under 1A too, since it flows through J5 when the panels are dark.
• No keying between functions: J1–J6 are the same 2-pin type, so a battery lead fits a solar socket. Check the silkscreen before plugging in. The switch headers take a different plug, so they can't be mixed up with these.
• Battery polarity: "JST 1.25" LiPo pigtails have no standard polarity. Check that red goes to the pin marked + (pin 1 on J5) before connecting.
• Reading the marks: pin 1 is + on J1–J6. J1–J4 are rotated 180° from J5 and J6, so the marks read - J1 + on the solar inputs and + J5 - on the right-hand connectors.

Operating note: if SW_BATT is off while the panels are in sun, the charger sees no battery and VBAT pulses around 4.2V. Keep SW_LOAD off in that state.

Power monitor (INA219)

• Address: 0x40 (A0 = A1 = GND).
• Shunts: both are 0.1Ω, the same as common INA219 breakout boards, so the default 32V/2A calibration in the usual libraries (e.g. Adafruit_INA219) works unchanged: about ±3.2A full scale, 0.8mA resolution.
• Pull-ups: R8/R9 are 10k I2C pull-ups to the MCU's VCC. Leave them off if the MCU board already has pull-ups.

The MCU can't sense SW3's position. Firmware has to know which position is set, or infer it from the readings.

Testing

The signs match the expected convention: positive while charging, negative while discharging. The USB reading comes from the XIAO's own charger, so it doesn't test the CN3791. The sunlight reading is from SW3's SOLAR position: 4.56V is above a Li-ion cell's 4.2V and close to the 4.58V MPPT set point. It's a single reading, and longer-term results are still to come. These tests used a board with Micro JST 1.25 connectors on J7 and J8, so the pin-header version hasn't been built yet. In the sunlight test build, J7 and J8 are bridged with wire on the back of the board, so neither switch is fitted.

Fabrication

Download the package from the latest release. That release is v1.0, which has Micro JST 1.25 connectors on J7 and J8 and no polarity marks. The design in this repo is v1.1, still a work in progress, and it will be released with the next fabrication batch. The package is generated into output/fab/, which isn't tracked in git:

LCSC part numbers are only filled in where verified (D5–D8). Pick the rest in the assembler's part search, and check rotation and polarity in their preview. The PicoBlade headers, the J7 and J8 pin headers, and SW3 are through-hole parts.

Regenerating the package (after the board is final and DRC is clean):

OUT=output/fab
P=SolarNodeChargeController
kicad-cli pcb export gerbers --layers F.Cu,B.Cu,F.Paste,B.Paste,F.Silkscreen,B.Silkscreen,F.Mask,B.Mask,Edge.Cuts --subtract-soldermask --check-zones -o $OUT/gerbers $P.kicad_pcb
kicad-cli pcb export drill --format excellon --excellon-units mm --excellon-zeros-format decimal --drill-origin absolute --excellon-separate-th --generate-map --map-format gerberx2 -o $OUT/gerbers/ $P.kicad_pcb
kicad-cli pcb export pos --format csv --units mm --side both -o $OUT/pos-kicad.csv $P.kicad_pcb
kicad-cli sch export bom --fields 'Value,Reference,Footprint,${QUANTITY}' --labels 'Comment,Designator,Footprint,Qty' --group-by 'Value,Footprint' --ref-range-delimiter '' --exclude-dnp -o $OUT/bom-kicad.csv $P.kicad_sch
node tools/fab-package.js $OUT

Repository layout

SolarNodeChargeController.kicad_pro / .kicad_sch / .kicad_pcb   KiCad project
SolarNode.kicad_sym             project symbol library (CN3791)
sym-lib-table
tools/
  gen-schematic.js              generates the schematic (Node)
  place-pcb.py                  places footprints, labels, holes, outline (KiCad Python / pcbnew)
  route-pcb.py                  routes tracks, GND stitching vias and pours (run after place-pcb.py)
  make-diagram.py               draws docs/images/wiring-diagram.png from the board render
  fab-package.js                JLCPCB-style BOM/CPL, fab notes and Gerber zip from the kicad-cli exports
docs/images/                    images used in this README (snap/: photos from the SNAP v1.2 MakerWorld post)
CLAUDE.md                       design decisions and working notes

The schematic and the board layout are generated by scripts in tools/, and checked with kicad-cli ERC/DRC (including schematic parity). See CLAUDE.md for the full design rationale and workflow. Generated outputs (output/: BOM, reports, fab files) are not tracked.

Regenerating the design

The whole design can be rebuilt from the scripts. Run these from the repo root, with kicad-cli from KiCad 10:

# 1. Schematic (Node): rewrites the .kicad_sch, SolarNode.kicad_sym and sym-lib-table
node tools/gen-schematic.js
kicad-cli sch erc --format json --severity-all -o erc.json SolarNodeChargeController.kicad_sch
# 2. Netlist for the board scripts
kicad-cli sch export netlist --format kicadxml -o net.xml SolarNodeChargeController.kicad_sch
# 3. Board (KiCad's Python): placement + labels + holes + outline, then routing + GND pours (~5 min)
"C:/Program Files/KiCad/10.0/bin/python.exe" tools/place-pcb.py net.xml
"C:/Program Files/KiCad/10.0/bin/python.exe" tools/route-pcb.py
# 4. Check: expect 0 violations, 0 unconnected, 0 parity issues
kicad-cli pcb drc --schematic-parity --severity-all --format json -o drc.json SolarNodeChargeController.kicad_pcb

The scripts overwrite their output files. Once you edit the schematic or board in KiCad, stop regenerating that file (or port your edits into the scripts first).

Refreshing the images in docs/images/:

kicad-cli sch export svg -o docs/images SolarNodeChargeController.kicad_sch
kicad-cli pcb render --side top --width 1600 --height 900 --quality high --zoom 1.6 -o docs/images/pcb-top.png SolarNodeChargeController.kicad_pcb
kicad-cli pcb render --side bottom --width 1600 --height 900 --quality high --zoom 1.6 -o docs/images/pcb-bottom.png SolarNodeChargeController.kicad_pcb
kicad-cli pcb render --width 1600 --height 1000 --quality high --perspective --rotate "-40,0,-25" -o docs/images/pcb-iso.png SolarNodeChargeController.kicad_pcb

(The schematic export is named SolarNodeChargeController.svg; rename it to schematic.svg.)

After refreshing pcb-top.png, redraw the wiring diagram with KiCad's Python, which includes Pillow and NumPy:

"C:/Program Files/KiCad/10.0/bin/python.exe" tools/make-diagram.py