"Exotic" PCB stackup

Sure. You are almost certainly going to need

ground rogers high-speed track rogers high-speed track rogers

in the middle - you can't route anything that's even moderately complex with just one layer unless you use so many vias that the tracks won't look like transmission lines any more.

And when I was working with Gigabit Logic's GaAs and 100k ECL, it made more sense to route over -2V termination power planes than over ground planes, but this is nitpicking.

Buried "stripline" transmission lines are non-dispersive, unlike exposed "microstrip". They are narrower for a given impedance than their microstrip equivalent, which made it difficult to get an impedance much higher than 50R in FR4 epoxy glass. Most of the Rogers materials have lower dielectric constrants than FR4 which means you need a wider trace to get the same impedance, which ought to help.

-- Bill Sloman, Nijmegen

Yup. But ground on layer 1? Where are the parts?

We did something like that, with the Rogers off-center, and the boards curled up like potato chips. You could place a board on a desk and give it a twirl, and it would spin for almost a full minute. The symmetry thing really matters!

Are you sure you need blind vias? They're expensive, no?

At high layer counts, you're going to need very skinny stripline traces to keep the impedance at 50 ohms or more.

John

Did you try to hold a fan over it, see how fast it'll go? A prior spritz from the PAM can might spiff it up even more.

On the outside. Point being that in many cases (ah haha ahahah "cases") there are a lot of ground pins on large devices so they get connected to ground with no via, which reduces loop inductance and removes a lot of vias to free up inner layers. I can push easily for 3 mil spacing and 2 mil soldermask annular ring. This gives lots of copper. On smaller high performance parts, like Micrel flip-flops, there is a large ground paddle in addition to conventional ground pins anyways. Ground copper anyways, you see? Using blind vias permits via-in-pad construction and with the correct placement you can use filled or unfilled vias. Filled vias = in center of pad, or anywhere really unfilled vias = breaking out of pad, since some people feel that trapped gas can cause solder joint failure even though a 50% by volume air void is acceptable....

All in all, you end up with as much ground copper as you would have if it were inside, on account of all the via savings.

Yes! I'm surprised anyone would build such a board. Was there a waiver or a serious discussion beforehand? If the board is thick enough and the Rogers thin enough, you can do it with less than 2-3% warpage, as defined by the vendor.

Trivial next to getting all the parts to fit. And they're not that expensive. What's expensive with blind vias is the implied sequential lamination and three (or more) drilling cycles. If you get rid of the through hole vias you skip one drilling cycle, bringing cost down. If you can make the board 50% smaller you can put that many more boards on a panel, bringing unit cost down again.

This has happened before but I am looking into broadside coupled construction for future projects. A bonus I see so far is the "automatic" diff pair de-skewed routing of broadside coupled pairs. A problem is that I can't find how to get Allegro to understand broadside coupling. When I ask for diff pair routing it's always on the same layer.

Since this allows twice as many channels per layer, having a gnd-sig- sig-gnd construction means you actually save on layers.

I think I'm going in the right direction here. Wadda you think?

One approach that gets rid of the via stub reflections without requiring blind vias is back-drilling, where the parts of the plated via you don't need get removed with a drill bit. It's typically cheaper than blind vias, and works nearly as well. You do lose a little routability due having to have the vias go all the way through the board.

Cheers,

Phil Hobbs

What do you mean by broadside coupled lines?

========================== ----------- ----------- ==========================

or

========================== ----- ---- ==========================

or

----------- ========================== -----------

or something else?

John

The first one. As opposed to edge-coupled.

The above is broadside aka tightly coupled differential routing. With typical geometries approximately 90% of the electric field (coupling) due to the signal will be between the signal conductors, the other 10% to the adjacent planes.

Loosely coupled differential routing, typ 10% between signal traces and 90% to planes.

Uncoupled differential routing. Not generally recommended, but can work.

Tightly coupled or broadside is infrequently used due to the fact that you have to uncouple the traces at the ends in order to connect to component pins, forcing 2 mode conversions which can be avoided with loosely coupled routing.

Broadside routing has been extensively discussed on the signal integrity list, and anyone interested can read the pros and cons in the signal integrity archives, or sign up and ask further questions. (The S/N ratio of the moderated signal integrity list is about 40 dB better than SED; almost all posts are on topic, and I highly recommend it for anyone interested in the subject.)

OK, but yikes, the impedances will be low. What sorts of spacings?

John