Express PCB Plus and BGA's

[matthew180]

GARTHWILSON wrote:

Have you thought about putting parts on both sides?

I have, and I am doing that for this latest board. But I still need 4-layers. When using BGAs, it is really hard to not have parts on both sides, if only for all the bypass caps required for the BGA. It is also hard to go with just 2 layers unless you only plan to use the first 2-rows of pads on the BGA. But even then the, bottom would have to be almost entirely dedicated to power / ground routing. Even with 4 layers, I had to cheat and use the power and ground layers for signal traces here and there.

[GARTHWILSON]

All true; but I mentioned the parts-on-both-sides idea as a way to avoid going to a bigger board, not to reduce the number of layers. One thing I've never done so far is blind or buried vias, because of the added cost. I'm laying out a board now with parts densely populating both sides, and it would be nice to be able to make connections to the inner layers without bringing the via all the way out to the other side where components need that space.

[BigEd]

I found some PDFs talking about routing BGA parts, and indeed it seems that with 0.8mm ball pitch, tracks need to be 5mil/5mil or even slightly finer. (Don't much like mixing metric and imperial!)

https://www.xilinx.com/support/document ... -rules.pdf
https://www.nxp.com/docs/en/application ... N10778.pdf
http://www.latticesemi.com/-/media/Latt ... ent_id=671

For non-PDF resources:
http://processors.wiki.ti.com/index.php ... ndard_BGAs
https://electronics.stackexchange.com/q ... -8mm-pitch

[matthew180]

Oh yeah, being able to use blind and buried vias, as well as via-in-pad and laser-drilled vias would be fantastic! However, the cost of those features are prohibitive for a hobbyist. Heck, just going from 2-layers to 4-layers is a cost increase of about 40%. I do think those features will trickle down to us in the future, as commercial products like cell phones and computer motherboards demand even more extreme requirements on PCB houses. As I mentioned earlier, 5 years ago as a hobbyist I could not get boards will less then 8/8 mil trace/space. No I can get 5/5 and the small vias needed to do the 0.8mm pitch BGA I need. It is pretty cool. And I have even been successful at soldering the darn things!

@BigEd: yeah, unfortunately the mixing of imperial and metric is pretty much something you have to deal with all the time. I think the industry is going metric, but we are in a transition period that will take a while (probably a decade or more) to finally convert. But even then, you will always have legacy parts that are in one or the other. I prefer the metric, and I keep a text file open while I am working that has mm to mils, in single mil increments, from 1 mil to about 20 mil, then in 10 mil increments to about 100 mil. For the most common sizes, you really start to remember the conversions, like 6 mil = 0.1524mm, 5 mil = 0.127mm, etc. Those are the two I deal with mostly. I also note the power (current) capability of trace widths for when I'm routing power.

As for routing the 0.8mm pitch BGA, you can actually get away with a 0.1524mm (6 mil) trace between the pads, but the 0.127mm (5 mil) traces give you a little more room if you are doing a lot of traces or wide buses (i.e. memory interfaces and such). Some of the documentation specifies that you can get *two* 0.076mm (3 mil) traces between 0.8mm pitch pads! That is insane to me, but it will probably become the normal in a few years. I can certainly say it would have made my current PCB *much* easier to route! For now I try to stay at 0.1524mm (6 mil) or above, and only use 0.127mm (5 mil) when necessary, and I have not had any problems with the PCBs (all were done by OSHPark so far during my prototype stage).

[GARTHWILSON]

matthew180 wrote:

I do think those features will trickle down to us in the future, as commercial products like cell phones and computer motherboards demand even more extreme requirements on PCB houses.

It will probably be more a matter of the equipment improving. The market demand has been there for decades. I have a 2"x3" bare board here in front of me for a PCMCIA (credit-card sized—remember those?) hard disc from 1992, .032" thick, 6-layer, with .005" trace & space and blind & buried vias. The board house was qualified for .002"! How they can do that is beyond me; but I saw photomicrographs of them where the width of the trace was hardly any more than the thickness, IOW, the cross-section was virtually square. (1-ounce copper is 1.4 mils thick.) The sides of the traces were straight up and down, perpendicular to the board. Obviously the price would be high, even today.