PCB size reduction using blind/burried vias?

[Klaus Kragelund]

Hi

On a current product we are using standard vias on a 4 layer stackup on
a 100cm2 board

I have recieved a preliminary quote from the board manufactor that
using blind/burried vias on a 4 layer stackup will cost approximately
10-15% more.

So the question is, do any of you guys have experience of how much PCB
real-estate is saved going to blind/burried vias?

I mean - if 10% space is saved, then I get the technology of more
advanced vias for free, and I avoid a lots of holes in the ground/power
planes

Thanks

Klaus

 

[Brad Velander]

Klaus,
It would appear that you are looking at your costs in an unrealistic
manner. The savings of 10% space is not equal to 10% cost. For multilayer
boards, particularly multi-layer with blind or buried vias, your material
cost savings are probably closer to 1-2% cost for 10% size reduction.
(Unless that small size reduction allows the addition of further multiples
within a fabrication panel. Then you might save significantly. It all
depends on the size of your boards and how they fit into the fabricators fab
panels.)

Materials are typically cheap, the processing costs.

As for your question, there is no simple answer. It would take a lot of
details of the design to even start taking educated guesses. Like, number of
nets, components, component pitches, trace sizes and spacings, via sizes,
board size (as is), etc., etc.. Even at that it would be a guesstimate, only
you can know the existing circuit and how much you might expect to save in
board real estate.

My very very rough guesstimate, you wouldn't realize a significant size
reduction, assuming your design is now quite tightly packed and is forcing
this blind/buried consideration. How much addition routing space are you
going to realize on any one layer by the removal of a few vias, here and
there? If you only need a bit more room in some tight areas like around BGAs
(or other very tightly pitched components) , then you might have things work
out better with blind/buried vias.

But remember, on a 4 layer board you can't get both regular blind and
buried vias in the same design unless your fabricator is doing laser drilled
blind vias. I suspect they are not if they are only talking such a small
delta in pricing.

--
Sincerely,
Brad Velander.

"Klaus Kragelund" <klauskvik@hotmail.com> wrote in message
news:1167732059.282080.105920@k21g2000cwa.googlegroups.com...

Hi

On a current product we are using standard vias on a 4 layer stackup on
a 100cm2 board

I have recieved a preliminary quote from the board manufactor that
using blind/burried vias on a 4 layer stackup will cost approximately
10-15% more.

So the question is, do any of you guys have experience of how much PCB
real-estate is saved going to blind/burried vias?

I mean - if 10% space is saved, then I get the technology of more
advanced vias for free, and I avoid a lots of holes in the ground/power
planes

Thanks

Klaus

 

[Noway2]

Klaus Kragelund wrote:

Hi

On a current product we are using standard vias on a 4 layer stackup on
a 100cm2 board

I have recieved a preliminary quote from the board manufactor that
using blind/burried vias on a 4 layer stackup will cost approximately
10-15% more.

So the question is, do any of you guys have experience of how much PCB
real-estate is saved going to blind/burried vias?

I mean - if 10% space is saved, then I get the technology of more
advanced vias for free, and I avoid a lots of holes in the ground/power
planes

Thanks

Klaus

Another couple of things to consider is the convience provided by
normal vias when debugging and any concerns about reliability as blind
and buried vias are a lot harder to manufacture.

 

[qrk]

On 2 Jan 2007 02:00:59 -0800, "Klaus Kragelund"
<klauskvik@hotmail.com> wrote:

Hi

On a current product we are using standard vias on a 4 layer stackup on
a 100cm2 board

I have recieved a preliminary quote from the board manufactor that
using blind/burried vias on a 4 layer stackup will cost approximately
10-15% more.

So the question is, do any of you guys have experience of how much PCB
real-estate is saved going to blind/burried vias?

I mean - if 10% space is saved, then I get the technology of more
advanced vias for free, and I avoid a lots of holes in the ground/power
planes

Thanks

Klaus

If you have the space, there's no need for blind/burried vias. Are you
using 4 total layers, or 4 routing layers plus 2 power layers? If you
are using 4 total layers, it would suggest that your part density is
low and/or routing is simple which probably means you don't need
blind/burried vias. Where I have used blind/burried vias, I had space
and component position constraints and high density placement of parts
which led to using blind vias. If you are hand routing a board, it
makes the layout job harder. If you need space and aren't using 0402
capacitors and resistors, I suggest using smaller components before
going to blind/burried vias.

If you plan to use blind/burried vias, talk with your board
manufacturer about layer grouping rules before you commit to routing
the board. Better yet, send them a sketch showing the cross section of
the board and your proposed via layer grouping. They will give you
feedback about your layout that could save you time/money.

Use the simplest technology that will get the job done.

---
Mark

 

Hi Klaus,

I've been a professional PCB designer for over 20 years, and have heard
this question a few times before, and looked into it.

First, the amount of space to be saved is usually very small, perhaps
only 1-2 per cent. There is almost no case where the feasability of the
layout depends on such a small savings.

Since the cost of blind/burried vias can be quite a bit greater (of
course it's coming down as the years go by...) and also there are the
reliability and inspectability issues, I say avoid that technology if
at all possible.

I have found that the main things which keep layouts small are good
component placement and minimizing the number of vias. Increasing the
number of layers excessively, or using blind/burried vias isn't really
going to help much.

If you have a layout that you can't seem to complete, you might want to
hire another designer to consult with you on it. I use very accurate
mathmatical modeling to determine layout feasability, and define the
number of layers, vias, etc. It might only take me a few hours to
perform that analysis, and then you could either use it as proof that
the layout is impossible, or see what you would have to do to make it
work.

Best wishes,

Jean Lestrale

www.dakotacom.net/~lestrale

 

[Ben Jackson]

On 2007-01-02, Klaus Kragelund <klauskvik@hotmail.com> wrote:

I have recieved a preliminary quote from the board manufactor that
using blind/burried vias on a 4 layer stackup will cost approximately
10-15% more.

So the question is, do any of you guys have experience of how much PCB
real-estate is saved going to blind/burried vias?

If we're talking about inner vcc/gnd layers, then buried makes little
sense (short?) and blind is only going to help you on power/gnd vias.
One advantage of that might be freeing space behind a BGA to put in
caps. Other than that, it seems like a waste for 4 layers!

--
Ben Jackson AD7GD
<ben@ben.com>
http://www.ben.com/