when to go to a multiple layer pcb - Page 1
Forum section: electronics / projects

author: AndreasF
author_rank: Frequent Contributor
timestamp: November 25, 2011, 12:11:49 am
content: 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)

author: JuKu
author_rank: Frequent Contributor
timestamp: November 25, 2011, 07:51:32 am
content: 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.

author: jahonen
author_rank: Super Contributor
timestamp: November 25, 2011, 10:32:31 am
content: 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.Regards,Janne

author: Psi
author_rank: Super Contributor
timestamp: November 25, 2011, 11:23:48 am
content: 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 quicklyEDIT: sorry, i misread the topic as when to go to a multilayer pcb (from single)but info is still useful.

author: JuKu
author_rank: Frequent Contributor
timestamp: November 25, 2011, 11:51:02 am
content: Quote from: jahonen on November 25, 2011, 10:32:31 amRight. 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.

author: EEVblog
author_rank: Unknown
timestamp: November 25, 2011, 12:14:03 pm
content: Without knowing the exact details, that layout looks ok, and will likely work just fine.It's next to impossible to "guesstimate" when to switch, as every design has different requirements.Yes, you'll certainly be able to get better signal integrity with a 4 layer board, but if the 2 layer one works, and meets any EMC requirement you may have, then it's worth trying.You've almost answered your own question, as the two layer design is finished(?), and you really want to avoid 4 layer if possible. So best solution is take bet and build the 2 layer proto and try it.If you jump straight to 4 layer then you'll never know if the lower cost 2 layer solution would have worked, and you'll be forking out more money per board forever!But if the 2 layer board doesn't work, you've only lost the proto cost and some time. But upside is there is a good chance you'll gain cost savings forever...And as you don't mention edge rates or any controlled impedance traces, then I'm willing to bet that your circuit isn't that critical that would would warrant a 4 layer board.Dave.

author: AndreasF
author_rank: Frequent Contributor
timestamp: November 25, 2011, 02:06:34 pm
content: Many thanks for all the helpful replies and comments! Though I am not closer to any decision, I have a few more things to think about. Especially the edge speed seems to be something to consider (and I also hadn't even thought about impedance matching).At this point, it is a one-off design primarily for my own personal enjoyment, and I don't anticipate it going into any sort of production run (but who knows?). That's why I am more concerned with prototyping cost. From that perspective a 4-layer board actually sounds like the safer option. I'll just keep the current version tucked away somewhere, and if I later decide to try to reduce the cost I'll test the double-sided version.Thanks again!

author: deephaven
author_rank: Frequent Contributor
timestamp: November 25, 2011, 03:57:27 pm
content: Quote from: AndreasF on November 25, 2011, 02:06:34 pmPrototype costs can be a lot higher for a 4 layer board compared to a 2 layer one. Chinese companies like iTead Studio produce very low cost 2 layer boards and would be a cheap option for you.

author: mikeselectricstuff
author_rank: Super Contributor
timestamp: November 26, 2011, 12:50:53 am
content: Something else to consider is the development versus production cost tradeoff for your volumes.A 4-layer board will generally be easier and quicker to lay out, and have less chance of noise problems with high-speed and/or high power nets, and so may require fewer spins. For a low-volume product with a small to medium PCB size, 4 layer may actually work out cheaper overall.A 4 layer design will generally allow higher component density, so you may be able to reduce PCB size, which could at least partly offset the increased PCB cost , and possibly also reduce assembly cost with more boards per panel.

author: gregariz
author_rank: Frequent Contributor
timestamp: December 02, 2011, 05:41:40 am
content: I typically use Batch PCB at ~$2.5/sqinch for 2 layers and ~$8/sqinch for 4 layers. I finished a crazy 2 layer board recently with a 2 x 4 in footprint (8sqinch) that actually took me 10 spins to get all the impedance matching right across the board. It worked out cheaper I think on a 2 layer board in this case. IME most boards of reasonable complexity (unless you have layed out a very similar circuit before) will take a few spins simply to overcome spec sheets lies and obscura. If's its a large board or reasonably simple board... I generally prefer 2 layers for cost reasons, if not or you have quite a pin count then 4 layers is a good bet.

author: ejeffrey
author_rank: Super Contributor
timestamp: December 02, 2011, 11:43:52 am
content: Quote from: mikeselectricstuff on November 26, 2011, 12:50:53 amThis is a good point. Even on a simple small 2-layer board I will spend hours or days laying out the components and tracks and trying to optimize everything. The same board with 4 layers I would just place the parts with my first guess, draw in power and ground, and hit autoroute. The result will not be great, but very often it is good enough and almost always it will be close enough to be fixed up by hand in a short period of time. Of course, this only works because we only need to beat a well done 2-layer board. If you want to really optimize a 4-layer board it will take time as well.