Anyone that’s ever tried to put 75-ohm video onto a PCB stackup knows how high impedance will drive layer thicknesses.\u00a0 Most busses operate using 50-60 ohm impedance, which means you would typically use dielectric thicknesses of around 5 mils to achieve those impedances.\u00a0 But 75-ohm video on a PCB requires dielectric heights more in the 8-10 mil range.\u00a0 Not a big deal, but those greater heights\u00a0will require wider traces to meet the 50 and 60-ohm requirements for any other bus signals routed on that same layer.\u00a0 And also, the signals will require greater spacing\u00a0between them\u00a0for crosstalk control.\u00a0 So it would kill your routing density.\u00a0 Comparitively, if you had 60 ohms as your highest impedance on that layer, you can assign that a nice skinny trace width of 4-5 mils, and keep everything a lot closer together.\u00a0 If you ever had to route to\u00a0the old 150-ohm differential FibreChannel spec and were worried about route density, forget about it!<\/p>\n
Speaking of differential, 100-ohm differential pairs\u00a0often create\u00a0the highest impedance, and are very common nowadays.\u00a0 In order to maintain good differential coupling, you typically need a single-ended impedance of around 65 ohms.\u00a0 In other words, the impedance of a single trace in the 100-ohm differential pair would be 65 ohms.\u00a0 So that would typically get assigned to the skinniest trace width for a given layer, usually 4-5 mils.\u00a0 The problem with that is that the 100-ohm differential signals are usually in the multi-GHz range, and are therefore more susceptible to loss isssues.\u00a0 So using wider traces can help that, but then that drives up the widths of all the other traces on that layer, as well as necessary crosstalk spacing, and hurts your routing density.\u00a0 That is why you see some differential signals now using 85-ohm differential pairs, to allow for wider traces.<\/p>\n