Where to put the layers 4 eurorack - Page 1
Forum section: electronics / general

author: mongo
author_rank: Contributor
timestamp: March 15, 2016, 04:31:59 am
content: I have been playing around with eurorack synth module designs and I have a design that will require 4 layers to to the limited size. I have a silly idea to break from the normal internal power and ground planes just in the hope that having them on the outside may help avoid noise from neighboring boards. However with as more mixed board wide voltages than I typically use (+12, -12, +5) I may not be able to do so without blind vias which are not possible with the small batch service I use.While this is only an audio level board so I don't have to worry about the added propagation delay with stripline differential traces will there more issues because my signaling layer will be next to my audio layer compared to my typical logic, power, ground, signal method I typically use? (mostly due to the ease of troubleshooting and tracing and laziness)Note that I am playing around with some historical designs for mix buses that use differential signals internally, as you can tell from this post I am way out of my area of expertise so please call me out if having a balanced signal pair on the outside will negate any real advantage. I enjoy learning by mistake but a 3 week turnaround for PCBs slows down that learning curve.

author: Christe4nM
author_rank: Unknown
timestamp: March 16, 2016, 05:42:46 pm
content: Well first of regarding the stackup. There are some EMI guru’s, including Henry Ott, who have talked about putting the power and ground planes on the outside layers for a 4 layer board. It supposedly can be helpful to shield your inner layers from the outside noises.PCB Stackup - IntroductionPCB Stackup - Four-Layer BoardsIt does have practical implications though (you already mentioned one) and implications on board signal routing.Thebiggest issue in practice is access to your signal traces. Troubleshooting can be challenging. You will also find you have many more via’s when using SMD components, as you need them to get your signal traces to the pads. In that case you need to be careful that you don’t get slots in your ground plane where it needs to pull back from multiple vias.When it comes to any electrical signal, whether voltage/current, high power/low power: as soon as the frequency content gets above say 1kHz, the return current likes to stay under it’s ‘send trace’. Which is very helpful for us designers: the better the send and return current couple to each other, the less they present problems to neighbouring signals and circuits. Hence the importance of the ground plane. Especially digital signals benefit from this as the edges produce frequency content into several MHz or 100s of MHz depending on the rise and fall times. So whatever you do, make sure you route those signals directly next to your ground plane.Also, contrary to many design notes it is definitely not a good idea to split the ground plane into a digital and an analog section. The best way to get good separation and keep signal integrity / noise performance is to keep one solid uncut plane. Instead in your layout create ‘zones’ for each circuit part, similar to how a city might be planned.• Put your digital section close to the power supply. This way any residual nose on the power rails won’t cross other parts of the board.• Put you analog section further away. The most sensitive parts the furthest. Make sure not a single digital signal crosses the analog ‘zones'.• Make sure input and output connections to off board wires are all on the same side of the board for the same signals. Keep the input connection to a signal close to its output connector. A good layout can be ruined by having an input on one side and an output on the other side. Any noise coupling into the cables and entering the board will most likely travel all across your board. You don’t want that.• As for connections, if not shielded, provide filtering first right at the connector. Pull the ground plane a little back so the signal gets to the filter without coupling to the ground plane.Incidentally you can consider using two ground planes instead of a power and ground plane, see the 2nd link above.In this topic I linked a few resources that might help.Especially the first webinar is a good and relatively 'quick' overview of the matter involved.Hope this helps

author: mongo
author_rank: Contributor
timestamp: March 17, 2016, 04:28:26 pm
content: Thanks for the reply,My ground plane was a mess every which way I tried to lay out the board.I think my whole problem was I was trying to stay on 4 layers, looking into the info you posted and other links I am just going to need to move to 6 layers and use orthogonal paths to avoid a lot of issues around ground plane cuts and noise. I keep forgetting that the LQFP-52 DAC I am using to produce control voltages has a clock that is pretty fast and, while it is most likely possible it is beyond my skills to keep the design clean when considering the current flows with a 4 layer board.In my mind 4 layers is a lot, my typical boards are small MCUs or ancient ICs, Because I'm a caveman -- that's the way I think.

author: Christe4nM
author_rank: Unknown
timestamp: March 19, 2016, 04:19:13 pm
content: Well 6 layers is a lot in my mind too. I never had to use it yet and have only come across it on digital-heavy boards with many many signals. And it does add extra costs to your bare board you would try to avoid.Are you sure it won't be overkill? Of course I have no idea how large your circuit is and what is involved so I can only speculate. I'm just saying this as I found that while I was learning I tended to go into overdrive just to make sure I had everything covered, only to find out that my design wasn't even close to being so critical as I thought. It's easy to get the idea that every little detail is the most important, so try to get an idea first of where your design sits in that spectrum.What may help you is to identify which parts of your circuit are sensitive and which aren't. What are the highest frequencies you can expect? Hint: that are the harmonics from rising and falling edges, not the fundamental frequency. Also, what kind of interference do you expect from the "outside" world? I.e. incoming cables and nearby devices (I understand that your design will sit in a Eurorack between other synth modules.)? The better you know, the better you can estimate how critical things are or aren't.When it comes to a clock signal, make sure you route that first. On a single layer (no jumping layers) and with the shortest distance possible. There are rules of thumb about the spacing to nearby traces on the same layer to keep crosstalk to a minimum. If I remember correctly it's 5x the tracewidth of the critical signal (the clock), but don't quote me on that. Also make sure that clock signal has a solid ground plane underneath. This in itself will help tremendously in keeping the clock signal where it belongs. So that's at least one worry less.That said, if you have a limited size for your PCB and a relatively large circuit, you might indeed need to use more layers.Good luck!P.S. You could think of opening a topic in 'Designs and technical stuff' about Eurorack design and how to fit everything while keeping your signals clean. That part of the forum tend to have more view, so you might find people who have practical experience with your specific design environment.