0
\$\begingroup\$

The PCA9450B is utilized to power up the iMX8 Mini Processor chip, which incorporates multiple voltage regulators. However, I am experiencing issues with the output voltages on the output side, despite using the circuit outlined in the reference schematic attached here.

Upon reviewing the datasheet, I noticed a potential problem related to Buck_GND, GND, and EP. The datasheet specifies, 'Buck reference GND for BUCK1,2,3. It should be connected to the ground plane through a Via. Do not short to EP directly on the top layer.'

In my board layout, Buck_GND, GND, and EP are shorted on the same layer. Do you think this could be causing the problem?

I appreciate any assistance from anyone who can provide insights.

Regards,enter image description hereenter image description here

\$\endgroup\$

1 Answer 1

Reset to default
0
\$\begingroup\$

EP is the power ground that all return (power) paths of bucks are joined at, and AGND and BUCK_AGND are signal grounds.

The application schematic on p.55 clearly shows this distinction. The ground that the bucks' SR MOSFETs on the right half are connected to is named PGND and has the same GND symbol as EP whilst all other signal-related grounds have a different symbol. To the right of the EP connection, it's shown that these grounds are joined together. NOTE: I didn't read the entire datasheet so I don't know if it's indicated somewhere, but these grounds may have been kept separately at the chip level, meaning that it is your responsibility to join them "properly".

enter image description here

The main idea behind this is to keep the signal grounds clean. Because the power grounds carry switching currents and all are joined at EP, it may get "polluted". Tying the AGND or other signal grounds directly to the EP is to ask for trouble because there's a risk of having the signal grounds polluted as well.

See the simplified schematic below:

schematic

simulate this circuit – Schematic created using CircuitLab

The switching currents flowing through the EP pin will induce voltage due to the presence of the via parasitic. This voltage may be too small to measure, but it's there, and it has a lot of high-frequency components. Tying the signal grounds here will make the signal grounds fluctuate (i.e. dirty). This may cause regulation issues. The easiest solution is to connect all grounds to a big enough plane (presumably with the lowest impedance possible) having no discontinuities.

\$\endgroup\$
3
  • \$\begingroup\$ Thank you, Rohat. Understood VIA importance between two grounds. I've implemented the largest common ground planes on three inner layers. Although I've routed on the same layer and manufactured the board, I'm considering cutting the signal ground traces and reconnecting them elsewhere. However, I'm skeptical about the effectiveness of this approach, as using external wires may result in an even smaller area. \$\endgroup\$
    – Ram prakash
    Commented Dec 10, 2023 at 11:14
  • \$\begingroup\$ @Ramprakash flying wires sometimes may work, but sometimes may not. They won't carry large currents, and they may not introduce large resistances, but this is a switching converter and if the wires pass by these nodes then there might be problems. Still might be worth trying. Do NOT connect the wires to the output caps' negative pins because nothing will change. In any case you have to update your layout. There's a good layout example in the datasheet. \$\endgroup\$
    – Rohat Kılıç
    Commented Dec 10, 2023 at 11:55
  • \$\begingroup\$ Thank you @Rohat for your advice. I'm experiencing a potential difference of 0.03V between GNDD and GNDPWR. Could a poor ground connection be hindering the operation of my IC? I'm observing readings like 0.7V instead of 3.3V and 0.03V instead of 0.9V. The output from my PMIC is not meeting my expectations. Please provide your insights. \$\endgroup\$
    – Ram prakash
    Commented Dec 11, 2023 at 9:15

Not the answer you're looking for? Browse other questions tagged or ask your own question.