Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronic Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Register Log in

Connecting GND on multilayer PCB

Status
Not open for further replies.

ajhsu

Full Member level 4
Joined
Apr 4, 2004
Messages
204
Helped
4
Reputation
8
Reaction score
3
Trophy points
1,298
Activity points
1,701
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

Advanced Member level 3
Joined
Oct 6, 2004
Messages
751
Helped
109
Reputation
218
Reaction score
24
Trophy points
1,298
Location
Iran-Mashhad
Activity points
4,036
multilayer pcb side through hole

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

House_Cat

Advanced Member level 4
Joined
Feb 21, 2002
Messages
1,371
Helped
406
Reputation
812
Reaction score
98
Trophy points
1,328
Location
USA
Activity points
16,422
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.
 

ajhsu

Full Member level 4
Joined
Apr 4, 2004
Messages
204
Helped
4
Reputation
8
Reaction score
3
Trophy points
1,298
Activity points
1,701
Except cost, what's the performance difference btw them ? Thanks.
 

biff44

Advanced Member level 5
Joined
Dec 24, 2004
Messages
4,837
Helped
1,354
Reputation
2,704
Reaction score
1,031
Trophy points
1,393
Location
New England, USA
Activity points
36,528
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

Full Member level 6
Joined
Apr 6, 2005
Messages
394
Helped
114
Reputation
228
Reaction score
27
Trophy points
1,308
Location
Kansas City
Activity points
4,630
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

Advanced Member level 4
Joined
Feb 21, 2002
Messages
1,371
Helped
406
Reputation
812
Reaction score
98
Trophy points
1,328
Location
USA
Activity points
16,422
ajhsu said:
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.
 

Status
Not open for further replies.
Toggle Sidebar

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Top