Based on the influence of some signal integrity experts and my own intuition and simulation experience over the years in signal integrity, I am convinced that loosely coupled differential routing is usually the preferred method for routing differential pairs in a printed circuit board. First a quick definition of loose vs. tight coupling:
Loose coupling – the ends of the differential pair are spaced far enough apart that the differential impedance is basically unaffected by the spacing between the pair and is basically equal to 2 times the single ended impedance of each line. A reasonable rule of thumb for this is a spacing that is between 3x and 5x the distance to the nearest reference plane for striplines.
Tight coupling - the ends of the differential pair are spaced close enough together that the differential impedance is affected by the spacing between the pair and the trace width must be narrrowed to maintain a differential impedance compared to the width of a singled ended line that is half the differential impedance.
The major benefits of loose coupling are:
- maximum trace width for a given differential impedance in a given stackup (minimize skin effect loss)
- further minimizes conductor loss due to current crowding on the side of the traces facing each other
- ability to route around obstacles such as vias an break out of pin fields without worrying about maintaining constant spacing to prevent impedance changes (you don’t have to be as picky with the PCB designer’s routing, especially regarding length matching
The major benefit of tight coupling is:
- routing density (you can pack more traces into a smaller area)
A second minor benefit of tight coupling is that it reduces the differential mode EMI from the trace, however for differential digital signaling, common mode EMI is a much more dominant factor and tight coupling does nothing to help this . Note that lower noise immunity to crosstalk is not a major benefit of tight coupling. In PCB structures, agressors rarely couple equally to both ends of a pair and thus crosstalk is nearly the same whether it is tightly or loosely coupled.
In general, the benefits of differential signalling that do not depend on loose or tight coupling are:
- reduction in simultaneous switching noise (SSN) – equal and opposite currents into and out of a chip when the IO switches significantly reduce the power and ground bounce due to switching outputs
- tighter noise margins and lower voltage swings
- reduction of common mode EMI over single ended signaling
Some engineers are hard to convince (tight coupling for differential pairs is deeply ingrained in engineers minds, even though the context within which the ingraining occured is usually in twisted pair cables which have a completely different geometry and design constraints), so I have compiled some links to articles by Howard Johnson, a highly respected industry expert in signal integrity.
Here are links to each article along with descriptions (detailed citations are given at the end):
Article describing crosstalk effects in PCBs for diff pairs:
Article describing why loosely coupled diff pairs are okay:
Article describing how common mode radiation from diff pairs is the dominant effect so tight coupling beyond a 20 mil or so threshold does not provide much benefit:
Newsletter article describing all of the benefits of differential routing and why loose coupling is better than tight coupling.
 Johnson, Howard. December 5, 2008. “Visualizing Differential Crosstalk.” EDN Magazine.
 Johnson, Howard. November 13, 2008. “Differential Coupling.” EDN Magazine.
 Johnson, Howard. December 12, 2002. “Reducing EMI with Differential Signaling.” EDN Magazine.
 Johnson, Howard. November 11, 1998. “Differential Routing.” High-Speed Digital Design Online Newsletter. Vol. 2, Issue 30. [Internet, WWW, HTML]. Available: Available in .HTML format; Address: http://www.sigcon.com/Pubs/news/2_30.htm. [Accessed: 15 January 2009].