Connecting GND on multilayer PCB

[chihhao]

multilayer pcb connecting directly to plane

Which one you prefer to connect GND togegher on multilayer PCB ?
(1) Connecting all layers of GND by through hole (No blind/buried via)
(2) Connecting all layers of GND by blind via & buried via (No through hole)

Thanks a lot.

 

[hr_rezaee]

multilayer pcb side through hole

I think choice (1) is better because it is cheaper.

 

[House_Cat]

For connecting ground planes together, there is no advantage to using blind and buried vias. Blind and buried vias will substantially increase the cost of your board without any measurable performance improvement.

 

[chihhao]

Except cost, what's the performance difference btw them ? Thanks.

 

[biff44]

RE:blind/buried vias. Sometimes you do not want vias with RF (or even DC) on the bottom of the board. That is because many boards have the ground metal of the housing touching the back ofthe board. This is important for higher frequency applications (above 6 GHz), and for getting heat out of the chips packed in high density on the board. Also, some applications suggest you should have no RF on the board backside, like if you are trying to filter RF signals for compliance testing, etc, where your filter may be adequate but the board is leaking harmonics due to weird ground loop currents.

Another time you do not want RF vias poking thru the bottom of the board is if you are using a metal can RF shield on the top side.

Blind and burried vias are higher cost, and can be a yield issue at some vendors.

 

[madengr]

Don't forget that when you run a via all the way thru the board you punch a hole in the VCC power plane. Your power plane will look like swiss cheese even though the ground plane is solid. I like to use blind vias so the power plane is not affected much.

 

[House_Cat]

Except cost, what's the performance difference btw them ? Thanks.

A thru-hole via is physically longer, which translates to higher inductance. Since you are using more than one via in parallel, the overall inductance difference between thru-hole and blind or buried is so small you can't measure it.

Let's make sure you understand the terminology. A blind via is made from either the top or bottom of the board, and doesn't go all the way through. Using current technology, it isn't possible to make a blind via more than about 8mils deep. That generally restricts the use to connecting from top or bottom to one, or maybe two layers beyond the top or bottom, depending on dielectric thickness. They are most useful on boards with components on both sides of the board. You can use blind vias to connect top or bottom components without intruding on the component mounted on the opposite side of the board.

Buried vias can only be used between two symmetric internal layers. They are drilled before the board is completely laminated. They can be long or short, but they don't extend all the way through the board. They are most useful for high density routing, where you want to route between layers under top or bottom traces, components or features.

It isn't that blind, buried, or thru-hole vias are superior to one another for electrical reasons, but rather what they allow you to do with the physical layout of the board.

Because blind vias are laser drilled, and buried vias add several additional fabrication steps, both processes increase the cost of manufacturing. They also reduce reliability and repairability. If a thru-hole via opens because of plating or local lamination problems, it can be easily jumpered - there's no chance with blind or buried vias. If a blind or buried via opens, the board is trash.