Should you try and minimize via quantity?

Question

I have a 6.5" x 4.5" double sided board that is mixed analog and digital.

I have partitioned the analog and digital grounds from each other and have zero ohm resistors that bridge the two grounds together.

But my layout involves a lot of vias. When I looked at the drill output file, its about ~400 vias. The bottom traces are kept as short as possible so as to just allow routing on the top layer, but because of that, I have a lot of vias.

Is this common to have so many vias? Should I look to make longer traces to reduce via count?

Update Added top and bottom layers

Answer 1

For basic low frequency work vias are pretty much "meh". The only thing you need to watch for is when running larger currents - the vias tend to have a higher resistance, so dissipate more heat.

However, the interesting things start happening at higher frequencies.

Vias start to become antennae. They can radiate EMI like nobody's business. So for high frequency signals, keep the vias to a minimum.

And by "high frequency signals" I don't just mean if you're intentionally working on RF systems. Digital systems have some very high frequency components too. For instance, a 10MHz SPI bus - the clock is running at 10MHz, with harmonics at 30MHz, 50MHz, 70MHz etc (depending on slew rate of course).

Also you have the question of impedance to look at. A via has a different impedance than a normal trace, so if your circuit is impedance sensitive (if you are doing impedance matched traces, PCB antennae, etc) then you have to take the vias into account in your calculations.

So for general power distribution, vias should be noted and thought about. For high frequencies, vias are anything from frowned upon to down right no-nos.

Everything in between is pretty much irrelevant.

Answer 2

One thing to be aware of is that when you're doing very large scale production, or optimizing heavily for cost vias do increase board cost marginally.

The more vias, the more time your board has to spend in the drilling CNC.

Answer 3

For a two sided board the ground plane is best kept as intact as possible and if this means via count goes up then so be it. This is a generalism so it can change depending on the type of circuit. Having said that, 400 vias seems a lot.

EDIT due to OP showing pictures.

I see the artwork you've done but there is a lot more you can do to minimize the impact on the ground layer. Look at the following small section I copied: -

If the three vertical red traces (left of diagram) were routed closer to each other, the blue tracks that break the ground plane would be miniscule in comparison. You've got to try harder in to minimize the discontinuities in the ground. The vertical blue track could possibly stay as a red track and sneak around the two red traces it crosses. There are lots of examples on your PCB where improvements can be made and yes, don't worry too much about via count - EMI performance is more important.