Question about differential pair routing - Page 1
Forum section: electronics / beginners

author: fubar.gr
author_rank: Unknown
timestamp: September 29, 2014, 01:09:13 pm
content: What is the recommended method of differential pair routing when the two lines have to cross?

author: Simon
author_rank: Unknown
timestamp: September 29, 2014, 01:12:28 pm
content: do they need to be exactly the same length ?

author: Sebastian
author_rank: Regular Contributor
timestamp: September 29, 2014, 01:28:10 pm
content: If you have a double sided load you could put one of two parts you need to connect on the other side (if that doesn't cause additional trouble) and have one via in each of the traces to change sides.But if it isn't too critical just cross them.

author: sacherjj
author_rank: Frequent Contributor
timestamp: September 29, 2014, 01:48:43 pm
content: Length isn't as important during the route, but they should be the same at the ends. The accuracy depends on the speeds you are running.Make sure you don't get into thinking that signal travels down one line and back the other. Each trace of a pair induces an opposite direction current on the closest conductor it can. This should be a plane, rather than the other pair. This is important to consider, because if you need to cross, you need to switch layers. Make sure that you have a method for the current that will be induced on the plane to continue. The absolute best situation is that you run the layer change from one side of the plane to the other. The distance between the conductors and layers will be different with most stack ups, so you will have an impedance change, unless you alter the trace width to compensate. If you have to jump more layers, make sure to provide a via path for the ground plane (with capacitive coupling if the induced plane is also not ground.)I sat in on an eye opening class at APEX by RF engineers that changed my thinking about routing from the traces to the EM fields between traces and planes. Keeping that in mind helps you not make stupid mistakes that will compromise signal integrity and cause EMI (both are the same thing, really.)Don't worry about pulling them a little apart from each other to match length. The reason they are run close together is so the induced EM fields cancel out. It is more important that the lengths are close than the conductors run close the whole way.

author: Precipice
author_rank: Frequent Contributor
timestamp: September 29, 2014, 01:52:31 pm
content: Can you weasel out of it, and come in to one part from the other side?If it's just USB, there's often the space to do this reasonably nicely (well, more nicely than vias and layer hops). Less easy if it's HDMI or something else with a load of lanes.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: September 30, 2014, 12:01:13 am
content: Quote from: sacherjj on September 29, 2014, 01:48:43 pmYeah, the coupling between edge-coupled differential is marginal at best, like 20-50%. Imagine the impedance between each line and to ground, the equivalent impedances act like a triangle with roughly equal values (like 150 ohms or so). So you get your 100 ohms differential, but there's still a whole lot to ground.You can run differential traces independently, without worrying about the coupled distance. And you should, in that you should be aware that uncoupled lengths don't really matter at all. Crosstalk from unrelated traces is a bigger concern.As for crossing, ideally, every time a high speed trace passes over a plane split (in a multilayer board, e.g., entering a different VCC domain) or through vias to the other side, that crossing should be accompanied by a bypass cap across the split or between layers, as near to the signal via(s) as possible. (And yes, that means a bypass cap from VCC1 to VCC2 -- you can do each one to ground, but you get a longer loop.) In practice, the effect is so marginal that it's nearly undetectable in TDR, because the plane-to-plane coupling is way better than the trace-to-plane coupling.Differential has an advantage here, because as long as the signals are time delay matched, the up and down transitions cross the underlying discontinuity in an 'equal and opposite' fashion, so there is very little coupling indeed.And to be perfectly clear, I mean a gap between planes on a given layer (perhaps between 3.3V and 2.5V supplies between different areas), with contiguous plane (ground?) on another layer 'supporting' that transition. Not a complete gap through all layers, which is generally a Bad Idea.I'm also assuming that the split occurs in the layer nearest the signal traces; in a 4-layer board, you might have a completely solid ground but gaps in VCC, so one routing layer (top or bottom) will encounter a situation like this. With many layers, you might have the luxury of a plane for each, and not need gaps at all.Tim

author: tggzzz
author_rank: Super Contributor
timestamp: September 30, 2014, 07:30:34 am
content: Quote from: fubar.gr on September 29, 2014, 01:09:13 pmWhy are they differential? Because they are high-speed digital or because they are low-noise analogue?