I would like to know the effects of stubs and vias in high-speed PCB designs, and how to eliminate or reduce them.
The stubs can be socket stubs and the like.
Vias are a necessary evil but how can they be made more transparent to the high-speed signal?
The speeds I am talking about range from 400Mhz to 3Ghz (Digital and Analog).
Thanks for your interest in High-Speed Digital Design.
Regarding socket stubs, there isn't much you can do except to not have them (i.e., don't use sockets). I know that's impractical in many cases.
- Blind vias are smaller and have less effect than full-sized vias.
- When your trace is adjacent to one power (or ground) plane, and then jumps through the via to run adjacent to a different power (or ground) plane, place a bypass capacitor nearby to help returning signal currents follow along (they have to jump from plane to plane too), or
- Better yet, route your trace so that it pops back and forth between two planes which carry the same DC potential, and then use a plane-to-plane via near the signal via to help returning signal currents jump from plane to plane, or
- Even better than that, route your trace so that it pops back and forth between the two sides of a single plane. In this case no special return current provision is necessary.
The use of both-ends termination (series and source termination used together), often combined with differential signaling, will produce a circuit with a great deal of immunity to the reflections caused by vias. Simulate this one to see the difference. To make use of this idea, you will of course need a differential receiver with good sensitivity.
Dr. Howard Johnson