Differential pair trace gap change: sudden vs. gradual

Question

I'm finalizing the routing for an eighteen-layer board that requires many, many differential-pair traces to run at speeds up to 16 Gbit/sec. (FYI: 100 Ω impedance, Isola I-Speed cores and prepreg.) These traces come from an MPSoC (BGA) with TX/RX pairs at 100 Ω impedance. All vias must be through-hole.

My design constraints limit me to roughly 3 mil trace gap while routing under the MPSoC due to the through-hole vias, then spread out to roughly 6 mil when the trace gap is no longer limited under the MPSoC.

I'm having trouble deciding whether my differential-trace pairs should spread out suddenly or gradually. I've read that in high-speed designs, trace width (not trace gap) will gradually fan out right before a pad to the pad width in order to minimize the sudden impedance change, similar to a tear-drop effect. Though taking this notion and extending it to trace gap seems logical, it poses two questions:

1. Is this reasoning even correct? A specifically unnamed eval board with trace pairs running at much higher bandwidth than mine (see below) employs a "sudden" gap-change, regardless of whether the trace pairs are A) "regular" high-speed using 45° bends, or B) "super duper" high speed and requiring curved traces.

2. What is too large of a differential-trace pair length to be changing the gap? If my reasoning is correct, there is no maximum "change in gap" length, but this doesn't feel right intuitively.

Here is an example from the aforementioned eval board, with the sudden trace gap-changes circled in red.

Here is an example of my board, with sudden changes marked in blue and the gradual changes marked in green.

Could someone please advise on the better strategy for this situation and explain why either the sudden gap (ergo, impedance) change or the gradual gap (impedance) change works better?

Answer 1

A couple of things first:

• When you change the gap, you also have to change the trace width to obtain the same impedance.
• I suppose a gradual adjustment would be ideal, but for every point in this transition area, the trace width and gap have to be such that impedance is alright. It will not lead to a straight fan type pattern, but complicated bent patterns.
• If you are not willing to properly design this long transition pattern that has the right impedance everywhere, the next best thing is directly jumping from the old width and gap to the new width and gap, which will cause approximately constant impedance. The length of impedance mismatch will be very short and not deter wave propagation that much.

Could someone please advise on the better strategy for this situation and explain why either the sudden gap (ergo, impedance) change or the gradual gap (impedance) change works better?

There is no impedance change if done right. Note how they narrow the trace width in the eval board when going from the two single lines to the tight diff-pair. This is done to get the same impedance before and after the change. They were not motivated to design a gradual change as explained above. So they went for the sudden step change. Apparently, it is good enough in that application.

Answer 2

More of a reference than an answer, but, According to IPC-2223E (Sectional Design Standard for Flexible/Rigid-Flexible Printed Boards)

"The conductor pitch for differential pairs used for controlled impedance should be kept constant along the length of the conductor to avoid unwanted signal noise / signal mismatch."

I expect this is generally applicable, rather than just being good-practice for flexi-rigid PCBs.