Via geometry parameters for controlled impedance in high frequency PCB

Question

I'm making a PCB with some high frequency striplines where impedance control is needed. After calculating, the track width according to my stack layer is 0.62 mm. I'm using blind vias to avoid any kind of stub due to excess copper.

I'm aware that vias are relevant in terms of return and insertion loss in high frequency design. After reading some literature I found some inconsistencies.

• Some places say that the via should be as small (and short) as possible to reduce inductance.
• Some others say the via diameter should be the same as the width of your track so as to have similar geometry to maintain the impedance. As I understand it, via diameter is via hole + crown. I'm not clear if just using 0.62 mm via diameter, the via hole diameter is not important and I can use 0.1 mm or 0.5 mm or any other as long as is less than the via diameter of course.

Which is the correct approach and what relevance does the diameter of the hole have to the overall diameter of the track?

I'm using Rogers substrate. The design is up to 5GHz but it is a system that sweeps from lower frequencies. Every dB in the final SNR is really important for the final application.

Answer 1

If you're working at 5 GHz with Rogers material, and return loss S11 is very important, then either

• do not change layers with an RF track or
• design the whole track layer change area as an RF transition, of which the via diameter is one of the least of your worries

If the RF track changes layer, then either they are referred to the same ground plane, or to different ones.

If they are referred to the same ground plane then they will change height, they will also need to change width. This will introduce a capacitive discontinuity. With the right design, you can introduce a sniff of inductance to turn it into a well matched lowpass filter, by either using a thin via, or relieving the ground plane back from the track judiciously.

If they are referred to different grounds, then you will need to make sure the RF current moves from ground to ground with minimum added inductance. Then you can design the rest of the transition as above.

A 3D RF solver would be useful to visualise just how much violence is occuring to the current flows as a result of the layer change, which will help you with tuning it up.

If you're working at 5 GHz with Rogers material, and through transmission S21 is very important, then you don't have so much of a problem, because you can get quite significant reflections from a single discontinuity with very little impact on the through gain.

If you have two or more bad matches at the right (wrong!) spacing, then resonance between them at specific frequencies can build up to serious through problems. As you've specified a swept measurement, you probably will find the resonant frequency.