Is the grounding on the PCB correct?

[tiger80]

Hi
I'm an amateur. I'm designing my own DC/DC converter based on the TPS54560. Check if I've laid out the grounding on the PCB correctly.
Thank you in advance for your comments and suggestions.

[thm_w]

Looks OK to me.
Maybe C13 can be further back from the connector to avoid cracking, but unlikely you'd actually see that issue.

[thermotto]

Just some things that popped into my head:

• Add thermals to the pads for the through-hole components to make soldering easier.
• The bottom left mounting hole appears to be connected to a ground plane, but the other two holes on the right are not. Is this intentional?
• Also, on the bottom left mounting hole, the connecting trace has an acute angle where it meets the ground plane. I don't know if it's still relevant or not, but I used to read that it's best to avoid angles less than 90 degrees since etching chemicals could pool at that spot and etch deeper than desired. It's probably easier to just expand the plane to cover the hole instead of connecting it with a trace.

[thm_w]

Just some things that popped into my head:

• Also, on the bottom left mounting hole, the connecting trace has an acute angle where it meets the ground plane. I don't know if it's still relevant or not, but I used to read that it's best to avoid angles less than 90 degrees since etching chemicals could pool at that spot and etch deeper than desired. It's probably easier to just expand the plane to cover the hole instead of connecting it with a trace.

Angles are not an issue, but your other advice is good.

[jovelyngentallan02]

The ground pour looks reasonable, but with a switching converter the critical issue is loop area, not simply having plenty of ground copper. Keep the input ceramic capacitor directly between VIN and the IC ground/PowerPAD, and make the high-current loop through the IC, catch diode and input capacitor as short and wide as possible.

Also:

Keep the SW copper small and away from FB, COMP and RT/CLK traces.
Take the feedback divider’s ground from the quiet output-capacitor ground, not from the diode’s noisy return path.
Connect the exposed PowerPAD firmly to ground with several thermal vias.
Keep the output capacitor close to the inductor and diode return.
Decide consistently whether mounting holes are grounded; chassis mounting holes should not be connected accidentally.

I would compare the placement and routing directly against TI’s TPS54560 datasheet example layout and evaluation-module layout. Those are better references than judging the ground pour alone.

[tiger80]

Hi. Thank you for your valuable feedback. I've reduced the amount of copper to a minimum for the SW signal. In version 3, I've relocated the output connector and moved the GND of the output capacitors closer to the diode pad. The IC pad is connected to the top layer with vias. There's some exposed copper on the top layer in this area, and there will also be a heatsink there. Which version is better, version 2 or version 3?