Electronics > Projects, Designs, and Technical Stuff

when to go to a multiple layer pcb

(1/3) > >>

I'm currently working on a slightly more complex pcb design and I am wondering if there are any rules-of-thumb or guidelines to decide when it's necessary to go from a double-sided board (with most signal and power traces on the top, ground plane on the bottom) to a 4 or more layer board with internal power, ground and/or signal layers.

The current design is double-sided and I tried to optimize the routing as much as possible (high-frequency signals short and only on one layer, a single uninterrupted ground area to reduce return path, thick power traces etc.), but because there are multiple supply voltages involved there are a few power traces on the bottom layer that 'penetrate' (for lack of a better term) into the ground plane and thereby slightly partition it (see pic). Therefore I am worried that once the board is manufactured and assembled I will find signal integrity or other issues that could have easily been avoided with a multi-layer design. Of course going to a 4-layer board would increase the cost of prototyping/manufacturing quite a bit, so I'd like to avoid it if possible.

In essence, is there a way to "guesstimate" how essential more than two layers are for a design?

(Some additional info: The design is almost entirely digital logic; a small analog portion is tucked in the upper right corner with the separated ground area, with the 'gap' between two bridged by a codec IC on the top layer)

My rules-of-thumb:

-First and foremost: every design and factory is different, at least somewhat. Don't just do 2 or 4 layers just because that's how you've always done it, talk to your factory or PCB supplier.

-In prototyping, you can make shortcuts that are not good for real production. Your board, as it is, looks just fine for a prototype. Besides, in prototypes and really small quantities, the bare costs don't matter that much, the setup costs dominate.

-For real production, you want to be real confident about your design and spend some extra effort for that. For example (disclaimer: without knowing what the circuit does), I don't really like your power supply routing; the return paths are not necessarily clear, straight and shortest possible, and traces on the edges are more susceptible for noise. Also, I don't like the small area with tight routing. I'd try to split that up so that the ground flows between the traces, and take the long lines (assuming I'm not looking at a differential transmission line) to the top layer to make the plane more solid. In other words, rather than 3" tracks in the plane layer, I'd aim for 1" on bottom, 1" on top, 1" on bottom. Also, there are several places where moving a component or a via just a bit would allow the plane to flow around and between tracks, vias and parts. And btw, the 3v line about one third from bottom left corner has some sharp V angles, not something you want to do in quantities.

-When the design is noise sensitive (audio, measurement circuit) or high speed logic, it needs a solid ground plane. Sometimes, you can arrange "solid enough" plane (see above), but if you can't, multilayer it is.

-For me, 4 layer board is about 30% more expensive than a 2 layer board. In my designs, almost always using more layers allows much more tighter routing, resulting in more than 30% reduction in board area. Therefore, in most cases a 4 layer board turns out the be cheaper than 2 layers, and I'll get a unbroken ground plane as a bonus. Talk to your factory, they'll know the pricing with your quantities.

-Another issue you want to ask your factory about is single or two sided component placement. Single sided is cheaper, but needs a bigger board, and that cost more. The money involved in this and the above tradeoff is big enough that you want to ask. For me, that is several dollars per board. Ten dollars per board on a thousand boards is worth a few days of extra work, but for ten boards, not.

Old rule was that if one has faster edges than 5 ns, then a multilayer board is recommended. Also, if you need impedance matching with sane track width with normal board thickness (1.6 mm or so), then the multilayer board is only option.

Another thing to consider is that if you must pass EMC etc. requirements. You might find only after several months of struggling, patching and re-spins that you really need the multilayer board to pass the tests.


I think the question should really be "when to go to a single layer board"

Pretty much everything is worth having 2 layers or more.
Power supplies are one possible exception though, since they often revolve around clear cut sections,  input, output, filtering etc. which all link together in a line rather than a star like digital logic/micros. So there is less need for jumpering around the circuit.

Trying to put a digital bus on a one layer board brings forth rage quite quickly :P

EDIT: sorry, i misread the topic as when to go to a multilayer pcb (from single)
but info is still useful.


--- Quote from: jahonen on November 25, 2011, 10:32:31 am ---Old rule was that if one has faster edges than 5 ns, then a multilayer board is recommended.

--- End quote ---
Right. I forget to mention that almost everything digital counts as high speed nowadays. It is not the clock frequency that counts, but edge speed. You need a good plane, and almost always, that means 4 or more layers.


[0] Message Index

[#] Next page

There was an error while thanking
Go to full version