Third-party CAD models, symbols, and footprints under lib/ retain their respective upstream licenses. See lib/README.md.
This repository holds the schematic and PCB layout files for the Sumodd mini-sumo robot motherboard, as well as documentation for the layout of the various components.
When a new iteration of the PCB is manufactured, the latest included commit is tagged with a
version number, e.g. v0.2.
The board has four copper layers, with a total thickness of 1.6mm.
- F.Cu — components, signal traces and power traces
- In1.Cu — GND plane
- In2.Cu — 3.3V power plane
- B.Cu — signal routing overflow
The PCB is powered by a 2s 7.4V, 25C, 800 mAh LIPO battery. This voltage is fed to a MOSFET transistor source, the gate of which is controlled by a SPST switch that connects the gate to ground when closed, and a pullup resistor that connects the gate to source when opened. The transistor drain feeds a 7.4V power rail on the top layer, which connects directly to the motor driver VM input. However, the MCU and other components want a stable 3.3V, so we use a MPM3610AGQV-P buck converter configured to step down the battery input voltage, to feed the 3.3V power plane on the third layer.
Datasheet: https://cdn-learn.adafruit.com/assets/assets/000/127/631/original/MPM3610GQV-Z.pdf?1707519066
The MPM3610 is implemented as documented in the typical applications sections of the datasheet, figure 12, to arrive at an output of 3.3V, while following the PCB layout guidelines in figure 10 (screenshot below).
- The EN (enable) pin is connected to IN (VIN) with a 100k resistor, to pull EN high when the device is powered.
- There is a 10 uF decoupling capacitor on the IN (VIN) pin, because the regulator switches a MOSFET on and
off rapidly (2MHz switching frequency), which leads to ripple currents. The capacitor maintains the DC
voltage from the battery, and provides the AC current the regulator demands each switching cycle.
- Note: a low-ESR ceramic capacitor with X5R or X7R dielectrics is recommended in the data sheet, and it should be placed as close to the IC as possible. It should have an RMS current rating greater than half of the maximum load current. Since the regulator will only supply the MCU, the sensors and some LEDs, it will have a low maximum load current, around 100mA.
- There is another decoupling 22uF capacitor on the output, to stabilize the DC output voltage, providing transient current when the load suddenly changes. Ceramic, tantalum or low ESR electrolytic capacitors are recommended, to keep the output-voltage ripple low.
- The FB pin (feedback) is connected to the tap of a resistor divider from the output to GND,
which is used to control the output voltage. The regulator adjusts the duty cycle to keep voltage
at the FB pin at the internal reference voltage (Vref), 0.798V. Since we want 3.3V, we need a
divider which leads to 0.8V at the tap when output is 3.3V. We use a 75k and a 24k resistor:
VOUT = 0.8 × (1 + 75k/24k) ≈ 3.3V. This matches the recommended values from the datasheet.- Note: the resistor divider should be placed as close to FB as possible, any noise on the trace can lead to incorrect adjustment of output voltage. Vias should not be placed on the FB traces.
- The AAM pin is pulled to GND through a 62k resistor, as recommended in the datasheet for 8V input, which puts the MPM3610 into power-save mode. In this mode it switches at a lower frequency during periods of low load, relying on the output capacitor to fill in the gaps, but during periods of high load it will transition to CCM (continuous conduction mode) and switch at max frequency. Read more about the modes in the datasheet, page 13.
- A LED with a 4.7k series resistor is connected from OUT to GND, lighting when the converter is powered and supplying the 3.3V output.
Note: the PGND, IN and OUT paths should have short, direct and wide traces.
Hardware development documentation (AN4206): https://www.st.com/resource/en/application_note/an4206-getting-started-with-stm32f3-series-hardware-development-stmicroelectronics.pdf
Datasheet: https://www.st.com/resource/en/datasheet/stm32f303c6.pdf
The microcontroller takes its power from the 3.3V rail, supplied by the voltage regulator. It reads all the sensors, and controls the motors via the motor controllers.
The hardware development documentation recommends:
- A multilayer PCB with a separate layer dedicated to ground, and another layer detected to supply (VDD), to provide good decoupling and a good shielding effect.
- The PCB layout should have separate circuits for:
- High-current circuits
- Low-voltage circuits
- Digital component circuits
- Circuits separated according to their EMI contribution. This will reduce cross-coupling on the PCB that introduces noise
- Unused I/O, clocks or counters should not be left free, they should be pulled high or low. This can be done through software by configuring the pins as GPIO output.
NOTE: for more detail, see the hardware development documentation section 5, where it also elaborates on which decoupling capacitors should be used and where.
For support components, we don't use an external oscillator, so we just need decoupling capacitors.
- For both VDD/VSS pairs, we have 4.7uF (X5R, 10V) and 0.1uF (X7R, 10V) ceramic 0805 decoupling capacitors.
- NOTE: these should be placed as close as possible to the VDD/VSS pairs, with the smaller one right between them. See example of this in the AN4206 doc, section 5.4.
- For VDDA, we have 0.1uF (X7R, 10V) and 1uF (X5R, 10V) ceramic 0805 decoupling capacitors, placed as close to the VDDA as possible,between VDDA and nearest VSS.
On this MCU, the BOOT0 pin should not float, and to boot from flash you need to pull the BOOT0 pin low. Therefore, we pull it low with a 10k resistor by default, but we also add an open 2 pad solder jumper, so that we can bridge BOOT0 to 3v3 if we need to boot with a bootloader. For more details on that, see section 3 of AN4206.
The PCB has one TB6612FNG motor driver, controlling two brushed DC motors, one on either side.
The motor driver has a max continuous current rating of 1.2A per channel, meaning per motor. It supports up to 2A for up to 20ms pulses at <=20% duty cycle, and up to 3.2A absolute peak for single 10ms pulses.
Datasheet: https://cdn.sparkfun.com/datasheets/Robotics/TB6612FNG.pdf
The TB6612FNG is implemented as documented in the typical application diagram of the datasheet, page 7:
- A 10k pull-up resistor from STBY to VCC, to always pull STBY high, which enables the IC, which saves us having to use a GPIO output pin to enable it from our MCU.
- One decoupling capacitor on the VCC pin, 0.1uF ceramic, to reduce noise from the voltage regulator, primarily due to fast and transient current demands of control logic, as well as trace inductance.
- Two decoupling capacitors on the VM pins, 0.1uF and 10uF ceramic, which takes
input voltage from the batteries directly. The motor is an inductive load which causes large, fast
current spikes when switching, and it can also feed noise back towards the battery. The capacitors
can supply the increased demand when current spikes, or absorb
back-EMF spikes when the motor
generates them: when the PWM switches it off, if the motor is driven backwards by a pushing
force or any other condition where the motor shaft is spun externally, turning it into a generator.
The TB6612FNG has built-in flyback diodes to protect the IC from this phenomenon, which redirect
spikes in current back into the supply rail, where the capacitors can absorb it.
- The datasheet recommends electrolytic for the 10uF cap, but it seems like overkill, it's big, and looking at prior art, adafruit uses ceramic for their breakout board, and sparkfun uses polymer.
NOTE: all capacitors should be placed as close to the IC as possible.
The final robot will have four analog line sensors, one digital IR receiver and three digital time-of-flight distance sensors. All of them will connect to the 3.3V power rail supplied by the voltage regulator. They will not mount directly to the PCB, the PCB will only have connectors for them.
Datasheet: https://cdn.sparkfun.com/datasheets/Sensors/Proximity/QRE1113.pdf Breakout board schematic: https://cdn.sparkfun.com/datasheets/Sensors/Infrared/QRE1113%20Line%20Sensor%20Breakout%20-%20Analog.pdf
For each sensor we have a three pin connector, which connects to the external breakout board with the sensors, which has the required components for the sensor itself. On the Sumodd motherboard, we just place a LED for debugging purposes.
The LED is connected in series with a 4.7k resistor from VCC to line sensor OUT. When reflection is low in the line sensor (no white line detected), the OUT voltage is high. When reflection is high, the OUT voltage is LOW. When OUT is low, there is a voltage difference across the LED, from VCC to OUT, which drives a current through the LED, lighting it.
A 330 ohm resistor was initially used for the LED, but the QRE1113 is based on a phototransistor pulling current from VCC, through a resistor to GND. OUT connects between the resistor and phototransistor, so as current increases through the transistor when IR reflection applies current to its base, the voltage across the resistor drops. The issue with the 330 ohm resistor was that it pulled more current through the LED and into OUT than the QRE1113 phototransistor could sink, preventing OUT from going lower than about 1.5V, significantly reducing the resolution of the signal. With a 4.7k resistor, OUT goes down to ~180mV with strong reflection, and the LED still lights clearly.
Datasheet: https://cdn.sparkfun.com/assets/c/8/5/c/8/tsop382.pdf
The TSOP38238 IR receiver is implemented as documented in the typical application diagram of the datasheet, page 1:
- A decoupling 1uF capacitor on Vs, to reduce input noise.
- A 470Ohm resistor on Vs, for protection against EOS, meaning protection against transient spikes of high currents or voltages beyond what the device is rated for. The datasheet recommends a resistor that is 33 Ω < R1 < 1 kΩ.
- A LED in series with a 4.7k Ohm resistor between OUT and Vs. Since OUT is pulled high when idle, and then pulled low in pulses when receiving a signal, there will only be a voltage difference across the LED when a signal is received, giving us a visual indication when a signal is received.
Datasheet and documentation: https://www.st.com/en/imaging-and-photonics-solutions/vl53l0x.html#documentation
For the time-of-flight ranging sensors, we simply have one 6 pin connector for each on the motherboard. It has pins for 3.3V input, GND, I2C SDA and SCL, as well as a DRDY GPIO external interrupt input which the sensor pulls low when data is ready, and an XSHUT pin, which we can use to reprogram the I2C address of the sensors, allowing us to run three on the same I2C bus.
I2C pullup and series resistors are placed on the Adafruit breakout boards we use for the sensors: https://www.adafruit.com/product/3317.