Editor’s note: This question was asked in response to Interference Technology’s recent webinar by Keith Armstrong. To view the webinar, click here.
Question: Should a ground moat be used across a signal transformer?
Answer: I’m assuming that we are discussing an isolating signal transformer with at least one side suffering from RF noise that we don’t want to cross over to the other side.
Yes, if the primary and secondary circuits are rigorously segregated (separated from each other) on the PCB, having a ground moat in-between them can help reduce the crosstalk between the traces and so improve the RF isolation of the transformer. However:
a) If the transformer windings themselves don’t achieve at least as much RF isolation (i.e. RF noise attenuation) as you need to achieve, a ground moat isn’t going to magically improve it!
It may be necessary to add a CM choke and/or other CM-attenuating devices such as shunt capacitors to the local RF Reference (see below), or reverse-connected CM chokes. Where balanced differential signals are used, additional CM attenuation can be achieved using center-tapped primary and/or secondary transformer windings, or center-tapped autotransformers.
b) The ground moat must have very low impedance at the highest noise frequency that we need to attenuate, let’s call it fmax. Assuming this is higher than a few MHz, our moat must be “RF bonded” (see below) to its RF Reference Plane (see below) with via-holes all along its length if it is thin, and all over its area if it is wide.
RF Bonding:
The general rule for RF bonding is that the bonds must be short, and make multi-point connections to an RF Reference Plane (see below) that are effective at up to fmax.
To be at all effective for frequencies up to fmax, the length of each bond, and the spacing between adjacent bonds, must be no larger than one-tenth of the wavelength at fmax (preferably a lot less).
In air, “one-tenth of the wavelength at fmax” is the same as 30/fmax, where fmax given in MHz gives the bond spacing in meters, and fmax in GHz gives bond spacing in millimeters.
But the dielectric constant, k (i.e. the relative permittivity) of the PCB material means that EM waves propagating inside the PCB have shorter wavelengths (actually 1/√k) than the same frequency propagating in the air.
Assuming a PCB dielectric constant of 4.0 (typical of FR4 above 1GHz and a good enough approximation above 100MHz), this means the via-holes that pin the moat to the solid ground plane must have a length and spacing no greater than 15/fmax (fmax in MHz gives via spacing in meters; fmax in GHz gives via spacing in millimeters).
However, “one-tenth of the wavelength at fmax” is simply the bond length and spacing to use to be sure that resonant effects aren’t going to cause gain when you are hoping for attenuation. To get good attenuation, RF bond length and spacing must be much less than one-tenth of the wavelength at fmax. The more attenuation we want, the shorter must be the bonds’ lengths, and the closer their spacing.
For example, if we want the moat that is the topic of this question to just about function as a moat up to 1GHz, then it should be via’d to the RF Reference Plane on a different layer of the PCB with vias spaced no more than 15mm apart (the PCB’s thickness is always going to be much less than 15mm, so the via length is adequately short).
But I would always recommend less than one-fifth of that (3mm), and why not 1mm – after all, vias don’t cost anything (well, not really).
There can even be an advantage in placing the RF Reference Plane one layer below (or above) the moat so that the via (RF bond) lengths are minimized. Where a moat trace is on an inner board layer, there can be advantages in using two RF planes in parallel, one on the layer above the moat, and one on the layer below.
RF Reference Plane:
A solid (i.e. no gaps or splits) copper PCB layer that is as large as possible, often covering the entire board area, and ideally extending beyond all of the components and traces on the board by as far as possible.
This is a much better term for a PCB plane that is used for EMC purposes, than “ground plane” or “0V plane”, because it helps avoid confusing EMC design issues with safety grounding or circuit DC potentials – confusion that has delayed very many design projects.
-Keith Armstrong
