Low layer count with blind/buried vias VS High layer count with regular vias - Page 1
Forum section: electronics / projects

author: fedimakni
author_rank: Regular Contributor
timestamp: March 12, 2025, 10:52:47 am
content: Hello,I am designing a PCB that contain multiple peripheral (USB super speed - ethernet - HDMI...)I am in the middle of the design phase and i reach 12L with regular via but still not able to completely route it.I was thinking about going to 14 or even 16L but at that time i was thinking what can be cheaper to manufacturer 14-16L with regular vias or 8-10L with blind buried viasCould you share your experience regarding the cost and design choice?Thanks

author: mtwieg
author_rank: Frequent Contributor
timestamp: March 12, 2025, 12:44:07 pm
content: IMO buried/blind vias are what you resort to in two cases:1. You have some super-dense BGA which is impossible to escape without blind microvias, even with an infinite number of layers (I'm guessing this isn't your situation, otherwise you wouldn't be asking).2. You have a very space-constrained board where vias are consuming a significant amount of real estate, which could be reduced by using blind/buried vias.If neither of those are true and you're just concerned about your ability to route all your nets, adding 2-4 layers is usually the cheaper option, IME. But if you have a good relationship with your fabhouse, it's worth asking them about it, doesn't hurt to try.

author: tszaboo
author_rank: Super Contributor
timestamp: March 12, 2025, 04:46:04 pm
content: You should request a quote from both options. Neither will be cheap, but the exact pricing always depends on your board house and quantity.

author: jbb
author_rank: Super Contributor
timestamp: March 12, 2025, 07:55:43 pm
content: You could also ask about High Density Interconnect (HDI) options; it’s another flavour of multilayer with blind vias.If you find yourself in the situation of having a a large board (eg to fit all the connectors) with only a small area of high density routing going on, it’s unfortunate because you’re paying expensive PCB prices for the whole area. In this situation you could consider splitting the design into a large cheap IO board and a small high-density module.

author: bson
author_rank: Unknown
timestamp: March 14, 2025, 08:27:01 pm
content: A long stretch of TH vias for things like a bus will always form a big obstacle; both electric and practical.Large QFPs can be routed underneath and placed closely: route from a pad to underneath, via, over to underneath the other package, via, and to its pad. The main obstacle is going to be the TH vias not just taking up a ton of space, but getting in the way electrically and for routing. They need to be spaced, which in itself makes things more complicated.The difficulty of escaping a BGA is not just a function of the pad count and pitch, but also the % of pads actually used. Sometimes going to a larger package with more pads and hence lowering the % connected makes iteasierto escape simply because it adds space and spreads out the connected pads. Sometimes this even permits removing layers. If the board house can do 0.2/0.25mm plugged TH-vias-in-pad then this is also very helpful.