Tell me more ×
Electrical Engineering Stack Exchange is a question and answer site for electronics and electrical engineering professionals, students, and enthusiasts. It's 100% free, no registration required.
up vote 4 down vote favorite

I'm trying to learn PCB design and, from what I've read and seen, there appear to be three different types of vias:

  1. Through hole - goes all the way through the board
  2. Blind - goes from the top or bottom layer to some layer in between the top and bottom, but not all the way through
  3. Buried - is between the top and bottom layers

It seems like most semi-complex boards I've had the opportunity to look at are 4-layer boards, and that usually one layer is dedicated to GND, another to VCC, and then the other two have traces. My question is what kind of via is most appropriate when trying to connect a pad or trace from one layer to the GND or VCC layers? I ask because I would have thought that a blind or buried via should be used, but it seems like most boards I've looked at use through hole vias and that there's just a stop around the via on the layers it's not supposed to be connected to. Is there a reason to use that method instead of using a blind or buried via?

share|improve this question
2  
Use regular vias that go all the way thru the board stack unless you have a good reason not to and understand the tradeoffs. Put another way, if you have to ask, stick to thru hole vias. – Olin Lathrop Jan 21 '12 at 20:21

3 Answers

up vote 8 down vote accepted

Blind and buried vias add a lot to the cost of a multi-layer board, and are only used on high-density, high-performance systems. The increase in cost is because the layers have to be drilled separately, assembled, and then the holes are plated. Blind vias are sometimes back-drilled (the unwanted plating is removed with a slightly larger drill from the back) which reduces the cost, as the layers are stacked before drilling.

share|improve this answer
4  
Just to add a bit to Leon's answer: Very little (none?) consumer electronics use blind/buried vias. They can't handle the cost increase and the benefits for those devices don't justify the cost. This includes PC motherboards that are super dense and super fast. I mention this because odds are that whatever you are designing doesn't require blind/buried vias. – David Kessner Jan 21 '12 at 17:42
Most likely, if you need blind/buried then you need a pro to do the layout for you. Make sure the PCB fab house is well experienced if you do need them; they are very difficult to get done right, especially when matching impedance for high-speed traces. – Aaron D. Marasco Jan 22 '12 at 0:50
up vote 4 down vote

Cost..

Here is a small example, I hired an inexperienced guy, he made a 4 layer PCB design, 30x50mm board. I sent to get a quote, I get a quote for 2K USD for 20 pieces, I naturally objected. They have said, this has buried vias. Later, I changed the design sent the gerbers back, price was 150$ in 5 working days.

Unless you have BGA package, don't use any via other than through hole.

share|improve this answer
1  
Even for BGA's, you don't need to even consider them unless the ball pitch is 0.65mm or less. Many 0.65 and 0.50 mm pitch BGAs can still be done without them. – David Kessner Jan 22 '12 at 6:05
up vote 0 down vote

Do not use Blind/Buried vias. You'll always find a cheaper way to finish your board without using them. That's what I used to do.

share|improve this answer

Your Answer

 
discard

By posting your answer, you agree to the privacy policy and terms of service.

Not the answer you're looking for? Browse other questions tagged or ask your own question.