8
\$\begingroup\$

I have read in some questions (for example: Via Stitching on 2 Layer PCB when top layer is not fully ground pour ), that stitching vias are useless when one's PCB only has 2 layers, however people do not mention the reason why.

As I understand it putting vias at close enough a spacing prevents a certain range of frequencies from travelling through your board, I do not see why I would need copper pours on both sides of my PCB for that to work. Intuitively I'd say I only need that periodic via conductive pattern.

I am currently designing a PCB (actually my first one ever), and only have a single cooper pour (ground plane) on my top layer, the bottom layer has power traces and other signal traces, and some ICs. One particular component works at a switching frequency of tens of MHz. I was wondering if I could stitch vias around it to confine possible EM radiation.

What I read on other posts seem to indicate it would be useless if I don't have additional layers with a "second" ground plane, is it really the case?

\$\endgroup\$
1
  • 1
    \$\begingroup\$ In your situation, what do you think the vias are going to connect to on the bottom layer? What you're describing are blind vias, which really don't do anything for EMC. \$\endgroup\$
    – SteveSh
    Jul 4, 2023 at 21:43

3 Answers 3

7
\$\begingroup\$

I think we should separate the informal terms "via stitching" and "via curtains".

Via stitching = keeping several ground planes together to reduce noise, minimize impedance/resistance, lead off ground currents etc. The aim is to reduce the ground paths as much as possible.

Via curtains = a technique in RF design from preventing emissions to go in/out of the multi-layer PCB through the sides, by placing a "curtain" of adjacent vias alongside it. The aim is to block higher frequency wave lengths - common along antenna paths where you only want the energy to go in one particular direction. It can be used for making the inside of the PCB a "poor man's Faraday cage" of sorts.

Note that the fundamental principle of EMC design is that emissions will enter/leave through any non-conductive material opening, in any direction or angle, as long as that opening's largest possible diameter in any direction is larger than the emission frequency wave length (λ = c/f).


As I understand it putting vias at close enough a spacing prevents a certain range of frequencies from travelling through your board, I do not see why I would need copper pours on both sides of my PCB for that to work.

Only from a certain angle and only at wave lengths larger than the distance between the vias. Radiated emissions travel in every direction. Epoxy and solder masks do not prevent emissions from going in/out of the board from the top or bottom; you need solid copper pour for that.

So if you have copper pour on top/bottom as well as a "via curtain" along the sides, you can block noise from traveling in or out from the board. Needless to say, this technique doesn't work well with a 2 layer board, since you can't really have solid ground planes then.

Grounded vias do block noise from the top/bottom direction too, but again only up to a certain wave length, depending on close they sit to another grounded via. And it probably isn't feasible to spam grounded vias all over a 2 layer design or you'll have a hard time routing traces.

One particular component works at a switching frequency of tens of MHz. I was wondering if I could stitch vias around it to confine possible EM radiation. What I read on other posts seem to indicate it would be useless if I don't have additional layers with a "second" ground plane, is it really the case ?

I'm not an expert of switching regulator design, but yes you should have a solid, dedicated ground plane directly beneath it and "hot loops" where the switching currents pass through should be surrounded with a via curtain. You'll only connect this power ground to the main ground at one particular spot; ideally close to where the ground pin of the board is located.

\$\endgroup\$
6
\$\begingroup\$

I've written comments on this or related topics before, e.g.
Signal integrity: ground plane vs ground traces between signals
which you may find relevant.

To better visualize and understand what's going on, I highly recommend understanding transmission lines. High frequencies travel largely as waves in the space between conductors, rather than as electron currents in the wire. Ground serves as a guide to confine those waves. A transmission line is such a confinement with consistent properties along its length. Confined waves mean less leakage to nearby stuff, or free space: this is what we need for EMC purposes, as well as for effective design in general.

So, the fact that you're already designing with traces largely on one side and ground on the other, handles a lot of confinement. That's called a microstrip transmission line. Now, the line is still exposed to space on one side, so not all the field lines terminate into the ground plane, and there is some radiation. But it's vastly reduced, by a factor of maybe hundreds compared to a trace the same length without ground under it. (Mind, this is a very crude and unqualified statement, and at best a ballpark figure, just to give some sense of the effect.)

As for the linked answer, for a little explanation, consider this:

Current flow diagram, crossed traces

This is approximately the current distribution around the structure, for current flowing right to left in the top horizontal trace. The image current flows under it in the microstrip configuration (red over green). The ground plane suddenly stops, and the current splits up, around the edges of the hole made in the ground plane. The greater distance between trace and ground (it might actually be less straight-line distance, but it's edge-on -- much lower cross-section) means trace impedance is locally higher (maybe 100-150Ω, whereas the microstrip might be more like 50-80Ω). More current flows along the top edge of the hole as it's closer, but current still flows around the bottom edge, and for the geometry here that's probably a 3:1 ratio or so.

The same is true in the middle (dotted line, image current induced in the fat vertical red trace), but those currents loop back around to the multi-dotted-line regions -- overlapping the green plane and inducing image currents in the plane edge in turn. Which is to say, you get eddy currents here. (Oh, I suppose I should've drawn those, too, now that I'm making a point of this...)

Note that both traces share some flux associated with this induced loop current. There will be some crosstalk as a result. The loop is also exposed to free space on both sides: it acts like an inductive loop in free space (I mean, still surrounded by in-plane ground pour, but that won't completely cancel out its field), and thus having a potential for radiation.

Making accidentally large loops like this -- by crossing traces erratically, say, while using little or no via stitching of top/bottom grounds -- is a good way to make a slot antenna coupled to the traces either creating the slot, or directly crossing over it.

The fact that current flows along the signal vias (vertically) makes very little difference; it's a short structure, adding a tiny length to the route, at a somewhat poorly-defined impedance (since the distance from conductor to ground varies along its length, and there's coupling effects between top/bottom pads through the PCB laminate; weird things like that). Via impedance effects can be directly visualized with ~20ps edges (time domain reflectometry, TDR), but for most low-microwave and lower applications, it doesn't matter; and for power purposes, the resistance and equivalent inductance suffice to describe them.

As for stitching vias:

Suppose in the above figure, the red vertical trace were ground as well, and stitching vias were placed as so:

Layout diagram, with stitching vias

In this case, the dotted lines between fat trace and ground pour, are shorted out, giving a wider current path in the middle span. This will reduce the inductance. (Assuming this structure is say 10mm across, I'd expect the vias to reduce the trace inductance by, oh, 2 or 3 nH maybe?)

We might further consider the case where ground fills the top layer, around (but not including) the fat trace. In that case, vias placed in all corners, flanking the crossing, ensures that any currents looping around the opening (realize the effect of negative space: two traces crossing on a 2-layer board necessarily causes a hole completely through both planes, and thus opportunity for crosstalk and radiation) follow the minimum path around that loop. You still have an opening, but it can be small enough not to care, at the design frequency and required emission/immunity level.

\$\endgroup\$
2
\$\begingroup\$

Tens of Mhz isn't particularly high. If you're switching a square wave you are going have some high harmonics thou. Keeping your vias very short will solve most problems. Soldering a shield can over the area involved will give you the benefit of a multi-layer board without the expense. This may or may not be necessary depending on your particular application.

\$\endgroup\$
1
  • 1
    \$\begingroup\$ Good way to limit harmonics is to have a series resistor at the driving end, to slow down the rise/fall times. \$\endgroup\$
    – jpa
    Jul 5, 2023 at 11:44

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.