Powerboard v1

Powerboard v1

A small 3.3 V supply module for battery-powered microcontroller projects: 4x AA NiMH in, regulated 3.3 V out, with an ultra-low quiescent current buck converter (TI TPS62842, 60 nA Iq), a switchable battery-voltage divider for an MCU ADC, a jumper for current measurement and test points. Breadboard format with two 1x04 pin headers 12.7 mm apart, like olmBoard (which uses the TPS62840 from the same family).

Board overview

Top view, switch at the top edge:

     ON <-- SW1 --> OFF  (actuator sticks out over the edge)
   Q1 R3              D1        F1
   R1 Q2                        J1  (battery: + upper pin, - square pad)
   R2 R4   TP1 (+BATT)
   C17     C14 C15 C2
   TP3 (GND)    U1                  TOP
                L1 R7
  J3 ●  GND     C1 C16       +BAT  ● J2
     ●  ADC                   GND  ●
     ●  EN      JP1 [BUCK|3V3] GND  ●
     ●  3V3                   3V3  ●
                       TP2 (+3V3)

Connecting it

Battery (J1)

2-pin socket, 2.54 mm pitch, for the plug of a 4x AA holder.

D1 blocks a reversed battery, so a wrong plug does no harm (the board just stays off).

Pin headers J2 / J3

Mounted from the bottom: plastic under the board, long pins down into the breadboard. Pin 1 is on the switch side. The labels are printed next to the pins on both sides of the board.

+3V3 on J2.4 and J3.4 is the same rail, after the current jumper JP1. All GND pins are the same. J3 EN only switches the battery divider; it has nothing to do with SW1.

SW1 on/off switch

SW1 is a C&K OS102011MA1Q, a right-angle (side-actuated) SPDT slide switch, through-hole. The footprint looks big because of its two large oval pads: they are the soldered legs of the metal frame that hold the switch mechanically and carry no signal. The three small pads in the middle are the contacts.

SW1 does not sit in the battery line. It drives the enable pin of the converter (net BUCK_EN):

• The slide direction comes from the C&K OS series datasheet: position 1 connects pins 1-2, position 2 connects pins 2-3, i.e. the slider always connects the middle pin to the outer pin on its own side. The ON / OFF labels are printed at the matching ends of the switch.
• Only the enable pin's input current flows through SW1, so its 100 mA contact rating does not limit the output. The load current goes J1 → F1 → D1 → converter.
• When OFF, the battery stays connected to +BATT (J2.1, TP1) and to the converter input. Take the batteries out (or unplug J1) for long storage; the standby current is far below the self-discharge of NiMH cells anyway.

Microcontroller, e.g. STM32WB Nucleo

If the Nucleo runs from USB, connect only GND, ADC and EN; never tie two 3.3 V supplies together.

The TPS62842 needs 3 ... 40 µF effective capacitance on its output (datasheet, COUT). C1 gives about 5 µF at 3.3 V; everything the load adds on +3V3 counts too, so keep the load's own capacitance below about 30 µF.

Measuring the battery voltage (EN / ADC)

R1/R2 (100 kΩ / 100 kΩ, 1 %) divide the battery voltage by two. Q1 (AO3401A, P-channel) switches the divider on and off at the battery side, Q2 (AO3400A, N-channel) lets a 3.3 V GPIO drive Q1.

One measurement (100 ms at 37 µA) costs about 4 µC, roughly 1 nA on average when measuring once per hour. The divider is off while the MCU is in reset or the pin is floating, so it never drains the battery by accident. While it is off the ADC pin sees 0 V, never more than the MCU supply.

Measurement sequence:

1. Set EN high.
2. Wait at least 65 ms (100 ms is comfortable): C17 (150 nF) charges through R1 ∥ R2 = 50 kΩ, τ = 7.5 ms; 8.3 τ settle to 12-bit accuracy.
3. Read the ADC: V_ADC.
4. Set EN low (or switch the pin to input / analog).
5. VBAT = 2 × V_ADC. This is the voltage after D1; the battery itself is about 0.2 ... 0.4 V higher (SS14 forward drop at the actual load).

Example (STM32 HAL, pin names are placeholders):

HAL_GPIO_WritePin(MEAS_EN_GPIO_Port, MEAS_EN_Pin, GPIO_PIN_SET);
HAL_Delay(100);                                   /* C17 settling, >= 65 ms */
HAL_ADC_Start(&hadc1);
HAL_ADC_PollForConversion(&hadc1, 10);
uint32_t raw = HAL_ADC_GetValue(&hadc1);
HAL_GPIO_WritePin(MEAS_EN_GPIO_Port, MEAS_EN_Pin, GPIO_PIN_RESET);
float vbat = 2.0f * raw * 3.3f / 4095.0f;         /* 12 bit, VREF = 3.3 V */

Current measurement (JP1)

JP1 is a 2-pin header with a jumper cap between the converter output and the +3V3 rail. It is not a power connector and has no GND pin.

The labels are on the top side, under the two pins.

• Normal operation: jumper cap on.
• Measuring: pull the jumper cap and connect the multimeter in current mode: red probe (mA / µA input) on BUCK, black probe (COM) on 3V3. The meter then shows everything drawn from +3V3 through the headers.
• Start in the mA range: a µA range has a large shunt resistance, so the start-up current of an MCU can drop the voltage too far and reset it. Switch to µA once the MCU sleeps.
• Not included in this reading: the converter's own 60 nA, the battery divider (only while EN is high) and the MOSFET drive. To measure the total battery current, put the meter in the battery lead.

Test points

SMD pads, 1.5 mm, for probe tips or small clips.

Battery voltage: TP1 against TP3. Output voltage: TP2 against TP3.

Ordering the PCB (JLCPCB)

Upload powerboard-hw/powerboard-v1/fabrication/powerboard-v1-gerbers.zip (Gerbers + Excellon drill).

The design stays inside JLCPCB's standard 2-layer capabilities: tracks ≥ 0.25 mm, clearance ≥ 0.2 mm, smallest hole 0.3 mm with a 0.6 mm via pad, copper-to-edge 0.5 mm, silkscreen text 0.8 mm high with 0.15 mm stroke. This is a bare-PCB order; the parts come from bom/powerboard-v1-bom.csv (JLCPCB assembly would additionally need LCSC part numbers).

Assembly and first power-up

Hand-solder footprints throughout, except U1:

• U1 (TPS62842, HVSSOP-8) has an exposed pad underneath that must be soldered to GND. Use solder paste and hot air or a hot plate. With an iron only, you can feed solder into the pad from the bottom through its two vias, but that is fiddly. Solder U1 first, then the SMD parts, THT parts last.
• L1 2.2 µH, 1008 (2520) size; C1 10 µF X5R/X7R ≥ 10 V; C2 4.7 µF ≥ 10 V; C14 22 µF ≥ 16 V.
• J2/J3 from the bottom (plastic under the board), JP1, J1 from the top.

First power-up, without a load:

1. Check with an ohmmeter: TP1–TP3 and TP2–TP3 are not shorted.
2. SW1 to OFF (slider right), jumper cap on JP1, batteries in.
3. TP1–TP3 ≈ battery voltage minus 0.3 V, TP2–TP3 = 0 V.
4. SW1 to ON (slider left): TP2–TP3 = 3.3 V.
5. EN to 3.3 V: J3 ADC ≈ half of TP1 within 0.1 s; EN open: ADC = 0 V.

Layout notes

• Signals on F.Cu, B.Cu is a solid GND plane, GND fill on F.Cu, stitching vias
• Converter laid out after the TPS62840 datasheet (DGR layout, fig. 63): C2 (4.7 µF) directly on VIN/EN and GND, MODE and pin 8 into the exposed pad with two thermal vias, VOS as a separate sense line to C1 away from the switching node, R7 on the VSET side away from SW
• Net classes: Default 0.4 mm, Versorgung (supply) 0.6 mm; copper-to-edge 0.5 mm
• Checks: ERC 0 errors / 0 warnings, DRC 0 violations, 0 unconnected, schematic parity OK

Files

powerboard/
├── README.md
├── powerboard-docs/            renders: 3D, top, bottom, layout, schematic
└── powerboard-hw/
    ├── powerboard-lib/         project library: TPS62842DGRR symbol, DGR footprint, STEP model
    └── powerboard-v1/          KiCad 10 project
        ├── powerboard-v1.kicad_pro / .kicad_sch / .kicad_pcb / .kicad_dru
        ├── sym-lib-table, fp-lib-table   (only ${KIPRJMOD}-relative paths)
        ├── schematic/          schematic PDF
        ├── bom/                BOM (CSV, grouped by value and footprint)
        └── fabrication/        Gerbers, Excellon drill, position file, gerber zip

Only the KiCad standard libraries are needed besides this folder.

Regenerating the outputs

From powerboard-hw/powerboard-v1/:

kicad-cli pcb export gerbers -l F.Cu,B.Cu,F.Paste,B.Paste,F.Silkscreen,B.Silkscreen,F.Mask,B.Mask,Edge.Cuts --use-drill-file-origin --subtract-soldermask -o fabrication/gerbers/ powerboard-v1.kicad_pcb
kicad-cli pcb export drill --drill-origin plot --excellon-separate-th --generate-map --map-format gerberx2 -o fabrication/gerbers/ powerboard-v1.kicad_pcb
kicad-cli pcb export pos --side both --format csv --units mm --use-drill-file-origin -o fabrication/powerboard-v1-pos.csv powerboard-v1.kicad_pcb
kicad-cli sch export bom --fields 'Reference,Value,Footprint,${QUANTITY},Datasheet,Description' --labels 'Refs,Value,Footprint,Qty,Datasheet,Description' --group-by 'Value,Footprint' -o bom/powerboard-v1-bom.csv powerboard-v1.kicad_sch
kicad-cli sch export pdf -o schematic/powerboard-v1.pdf powerboard-v1.kicad_sch

Status

v1, not manufactured or tested yet.