Re: PCB Layers


This sounds interesting. Are you using via-in-pad? Can you point
me to a good source showing how to use microvia's to improve BGA
routing? A quick Google search brought up lots of articles that
assume you already know the basic premise. Just at first glance
I would think that the inner portions of the BGA routing would
still require traditional techniques?

Regards,
Gabor

Hi Gabor,
Yes, I use via in pad. There's an article here all about it:-

http://www.sanmina-sci.com/Solutions/pdfs/pcbres/Impact_of_Microvia-in-pad_Design_on_Void_Formation.pdf

Void formation is seen as bad. My experience is otherwise. I've made boards
with microvias dead centre of the pad, offset from the pad, and Cu filled
microvias in pads. If there was a yield difference between these methods, my
production team and service guys kept quiet about it. (They sure moaned like
crazy when the QFNs had problems with pad size!)

I posted about this three years back, Google for "PCBs for modern FPGAs" in
CAF.

Here's a link to a picture of board I did then :-
http://www.fpga-faq.com/caf_pics/layer_1_2.gif

(Thanks to Philip for keeping it there!)

If you have 0.1 mm tracks 'n' gaps and make the BGA pad size 0.5mm, you can
get the first 3 layers out on layer one. Then work back from there, layer 2
can take perhaps 4 traces/mm. That lets you go 7 balls deep from the edge
without a through via. The powers and grounds use through vias. I try to
keep the through vias on the 'corner' of the destination pad nearest the
centre of the BGA, this facilitates the routing of the signal traces
outwards. The backside of the board can be covered with bypass circuitry as
there isn't the usual field of through vias filling this area.

(BTW., I did once use slightly bigger pads, but made the outer balls oval to
get the traces out. Again this made no detectable yield difference.)

The gap between layers one and two is necessarily small for microvias. This
is great news for SI; the laser drilled via has only a tiny inductance, and
the reference plane for layer 2 is the same as layer 1. Except in a microvia
board it isn't drilled with so many holes!

I've done many boards with microvias on one side only. (Keep the BGAs on
that side!) This way you can keep the price down. The stack up needs to be
symmetrical, but the distribution of planes doesn't. See the post from three
years ago for details.

Also, you can get a lot more stuff on a given sized board. Through vias get
in the way of mounting stuff on the backside of a board, the microvia
alleviates this problem.

And be prepared to swap pins on the FPGA when you do your layout. This saves
time in layout, and I know that PADS has a magic feature to assist in this.

In all, I find I get cheaper (fewer layers) and more compact boards, with
better SI, by using this technology.

HTH., Syms.





.

Relevant Pages

  • Re: PCB Layers
    ... Layer 1 Layer 2. ... me to a good source showing how to use microvia's to improve BGA ... microvias in pad will not be a very good option. ... I've used microvia in pad for 0.65mm pitch and it was very expensive. ...
    (comp.arch.fpga)
  • Re: PCB Layers
    ... microvias in pad will not be a very good option. ... I've used microvia in pad for 0.65mm pitch and it was very expensive. ... I spend more on the laser vias, but claw that back and more with the layer ...
    (comp.arch.fpga)
  • Re: How to remove old black lino tile backing from pine floor before sanding?
    ... moved but then I'm left with lower layer still. ... carpet pad off a concrete floor in the basement family room. ... Exterior sliding door was open, the water heater in the utility ...
    (alt.home.repair)
  • Re: How to solder BGAs with reflow oven, and what footprint to use?
    ... I've worked hard to avoid BGA ... It does not give a recommended footprint, ... If I want a via connected to a ball - can I put it on the pad ... Now - once I have my board made - how do I solder it? ...
    (sci.electronics.design)
  • Re: 320pin BGA Pin Layout suggestions
    ... From .75mm pitch on up you can do a conventional "Dog Bone" approach to fanning them out. ... then is to make sure your PCB vendor can do via in a pad. ... You may be able to squeeze row AC between AD and AB between AA and get it fanned out with say a .2mm drill in a .45mm-.50mm pad or some such away from the balls. ... To fan out a .5mm BGA this way you are going to need .083mm trace and space which is still way small, so again start with your fab house to see what they can do. ...
    (sci.electronics.design)