Why we need a pad around via in inner layer for analog board

via spacing guard ring frequency

hi all,

i've been asked to give a special instruction to pcb fabricator to have a small pad around a via in an inner layer. but i'm not sure why. this is a high frequency analog board. does anyone here know why? cheers!

akhmar

Re: pad around via

It will probably be a guard. Any RF leakage cannot get to the via because it is intercepted by the guard pad.

Git

Re: pad around via

You say the pad is around the via - do you mean it is an inner layer pad that is connected to the via? If so, the designer may have decided he needed a bit of capacitance in parallel with the via inductance. Capacitance would be so small that you probably can't measure it in the real world.

If the "pad" is really a ring around the via that is not connected to the via, or anything else, it may be a dampening ring. The current through the via would have to be relatively high for such a ring to be effective. The theory is that the magnetic field around the via would induce a current in the ring that gives rise to a field that counters the one originating at the via. This kind of thinking carried over from motor theory.

If the "pad" is a ring around the via that is connected to the signal return path, it is a guard ring. The idea of signal "guards" is a leftover from the old days of vacuum tube analog designs where the signals were ten's to hundreds of volts peak-to-peak on the same board with grid signals in the millivolt range.

All of the above are very questionable reasons to add extra copper on an inner layer. 1 - The signal would have to be in the GHz range for pad capacitance to even get into the range of calculation error. 2 - The signal current would have to be in the ten's of milliamps with a very fast rise time to make a dampening ring produce a noticeable bump on TDR. 3 - A guard ring is unnecessary if you space the vias and traces properly - if you have room for a proper guard ring in a solid state design, the traces and vias are probably far enough apart to make mutual coupling negligible without the guard.

In short - it sounds like somebody had some "thumbrule" that they applied without doing any real analysis or engineering. If they can't explain what they are doing with some hard math (or software modeling) they are just adding silly extras to the design.

pad around via

The pad was around the via that can reduce inductance effect, it could increase the performance.