Hi,
This is my first time designing a PCB and I was just wondering if I had done it correctly, I have traced my grounds through a microvia to underneath the board, where I trace each via to a common ground. I am not sure if I should keep this or I should pour the gnd instead. Any suggestions?
Thank you!
As a general rule, I always make a ground zone (or pour the ground) across the entire board on at least one full layer. So yes, make your entire bottom layer a ground zone.
Note that microvias (assuming you do actually mean microvias) are often very expensive and almost certainly not needed here. Use regular vias (made with drills) unless you know for sure you need microvias (often made with lasers).
Microvias are a fairly specialist fabrication item, and will drive the cost of your board up hugely. I’d just use a regular via size (drill and angular ring) that is within your manufacturer’s regular tolerance. And just put a ground fill over the entire underside of the board.
Ground Zone should either be much larger 3+ mm or a ground pour.
Vias should be regular vias but at least 2x the size of the default. No need to have small vias if you have the room.
I don’t know the function but it looks like some input protection. If this is the case, you want to have a 0.01µf as close to the input pin as possible. If the bottom is available for components, I would put these caps on the bottom right at the input pins directly to the ground zone.
I would also consider putting the ground plane on the top (with the components) and send the signals thru a via to your J3.
Reason: To shunt any RF or sharp spikes before they get onto the board traces.
Yes that’s exactly it, it’s supposed to be a potential divider ramping down 12V to 3V so that I can connect those signals to an MCU. I’ve taken notice of what you have said and added some extra capacitors to each input in series to the 90kOhm resistors, and utilised the bigger vias to send signals to the back of the board. I’ve also poured the ground. Is this a bit better ?
If it were my design I would certainly have all elements at top - you have enough room for it.
If you are allowed to sort the signals differently I would also try to have all signal tracks (except GND) at top.
From what I could see in the first screenshot, there already was a capacitor in each voltage divider parallel over the low voltage part of the divider, so it forms an RC filter for the inputs, or more important, it avoids high current peaks through the capacitors, which can upset the GND level. For more details, it’s best to post a screenshot of the schematic.
Meh, it depends on the application. If all SMT stuff is placed on the bottom, then it’s well protected from poking fingers and screwdrivers, and the top is free for labeling the silk screen.
When dealing with EMI susceptibility It is best to squelch it as close to the source as possible. Allowing the RF to get onto the PCB is a poor choice. That’s why they make “feedthru” filters.
I am aware of feed-through capacitors / filers. But in this case, I assume it’s better to put the capacitor behind the first resistor of the voltage divider. This way the capacitor current is limited and thus noise is not fed into the GND (plane). This is “just” an intermediate PCB, and it’s GND is probably just via some wire to somewhere else. It’s not a “hard” ground.
Those feed-through capacitors are mostly used with low impedance paths. I do not know the values of the resistors in the voltage divider, but it probably already has a high impedance.
I guess “best” approach here is to reduce the GND plane to the first resistor. (Seen from the “high voltage” side. This way, that resistor is the first barrier for RF noise, and what comes through the resistor is filtered by the low pas filter. This approach both filters EMI, and keeps the GND plane clean.
But we’re probably also overthinking it a bit here. It’s OP’s first PCB, and we have no idea of the environment this is supposed to live in.
Ok. All SMD at one layer and GND at the other.
I typically use SMB transil and then RC divider/filter.
