Proper PCB grounding? - Page 1
Forum section: electronics / beginners

author: SenSeS
author_rank: Contributor
timestamp: January 27, 2016, 08:25:26 pm
content: I saw Dave's video where he routes a PCB:(minute 29-35 are most relevant for my question). He starts (and suggests) to start with all signals, then power, and doesn't route ground but connects them all via the copper pour on the bottom layer. However, while searching around I came across the top answer of this post (which has quite a few upvotes)http://electronics.stackexchange.com/questions/15135/decoupling-caps-pcb-layout. Here he really suggests the opposite, to route ground and power first, then signals and more importantly, that it is considered bad grounding to have lots of ground connections in the ground plane, he advocates 1 per local net. Both people seem to be very competent at pcb design, yet their seems to be very contradictory. Could someone help clarify this please? Thanks!

author: uncle_bob
author_rank: Unknown
timestamp: January 27, 2016, 08:55:17 pm
content: HiActually it's even more complicated ....How fast are the signals on your pc board? It's not the clock rates, it's the edge rates that matter.How much power are you handling on your board? It's current more than voltage that will get you.What sort of signals are you dealing with? A board with nano volt level signals at 1 GHz will have different requirements than a "couple of volts" board at audio.What sort of budget to you have? If a four layer board is "ok" there are often easy answers to some of this. If double layer is already at max cost, you will need to work a bit harder.How dense is your board? Packing lots of stuff into a board *always* makes things more exciting.How much time do you want to spend? It's fairly easy to spend a couple of weeks on a board layout (full time weeks, not hobby time).How important are things like EMI and reliability? They are a very big deal in a commercial environment. They may or may not matter in a hobby design.So what's that all mean....If you have nanosecond rise time edges, you are dealing with GHz in your design. Solid ground is a real good idea somewhere in the stack up. A lot of modern digital stuff has fast edges. Will it work without solid ground - sure it will. Is going to work as well as it could work ... probably not.If this is a simple "audio" design, ground planes may not matter much at all. It's simply a matter of tying things together and moving on. Will a "toss it in" approach be perfect? Of course not, but it will do pretty well. It's also going to save you a lot of time on the board layout.So as with most real engineering questions the answer is ... "that depends". Indeed that is a direct quote from one of the "worlds best" level experts on this stuff when asked about pcb grounding.Bob

author: T3sl4co1l
author_rank: Super Contributor
timestamp: January 27, 2016, 10:55:47 pm
content: More grounding is almost always better. The best design approach for a 2-layer board is to surround all traces with ground pour, and stitch the top and bottom ground areas with vias, wherever possible. Each trace causes a break in the ground pour, on its layer; adding vias to short across the negative space solves this problem nicely. Thus, where two traces cross at right angles (top and bottom), you want to use 3+ vias at the inner corners of that intersection, so all the grounds are shorted together at that crossing.Proceeding in this way, you can build a 2-layer board that performs almost as well (in terms of high speed capability and electromagnetic susceptibility/emissions) as a full 4-layer board. The downside is, you want to ensure all signals are routed over ground, with a minimum of areas where traces/footprints occupy both sides (excluding a local ground), which means you're really routing over just one layer for the most part. So it can be wasteful on board area. But if you can afford the relatively low density, I mean, 2 layer board is *cheap* stuff...Tim