Wires in Ground Plane

So, your layout cannot be routed without putting wires on the ground plane. Bad! Very bad actually. (Unless your design is of a type that would not need a ground plane at all, but the plane is there for convenience only. Is true for about 0.001% of all layouts.) How to live with the fact that the ground plane is no plane any longer, but rather a patch work of "planies" (or mini planes)?

There are 3 domains to check in this case:

The thermal effect.

Let us start with that one, that needs the least attention - the thermal aspect. Not to state, that the thermal performance of your board does not need careful design, but to state that usually the ground plane is not used to conduct much heat. It is somewhere inside the multi-layer and can therefor dissipate only little heat. (Another approach, so called sandwhich boards are not considered here because they have a thick metal core that does not have any traces on it.) And even if you rely on your ground plane to conduct heat, the little planes usually can be made sufficiently large for that case. If you follow the design rules for the electrical effect you usually end up with a thermally good board, too. I wrote "usually" - never rely blindly on it - check it!

The magnetical effect.

The second effect, the magnetical, is a little bit trickier. By "magnetical" I mean the effects of currents flowing between the ground islands. These currents usually are invisible except in the worst cases. When confined to the unviolated ground plane they are called "ground currents" and not considered a problem in most of the cases - the ground plane was invented to minimize the effects of these currents. But as soon as you cut your plane with wires you might encounter them even at low frequencies of some megahertz. Why?

Let us consider an example of a lengthy board with an aspect ratio of, say, 1:8 (one dimension is eight times the other, eg. 2cm x 16cm). For this example we use a board with only one plane, just to show the principle. At the far ends you connect the wires for input and output, respectively. So, all the current from in to out must flow over the whole board along the longer side. Now cut the plane in the middle of the board, perpendicular to the flow of current, with a 1cm cut. Obviosly the current now "sqeezes" through the bottleneck of the 1cm left from the 2cm after the cut. Current desity is twice here, compared to the regions further away from the slot. At higher currents the copper may even be melted away. But what else happens?

Even with DC there is a magnetic field built up by the current - unavoidable, law of physics. On regions where the current flows through the full width of the board the magnetic field is distributed the same way. But at the narrow slit it is concentrated, flowing through a much smaller area. Thus the magnetic field is concentrated there, too. So, this creates not only a potentially thermal, but definitely a magnetic "hot spot" on the plane. And things become worse when we assume AC - and the higher the frequency the higher the impact on the rest of the board and its components. Imagine a case when you put a sensitive analog chip just above such a bottleneck and your ground plane has a current of some megahertz on it - absolutely usual in a mixed design. You can bet on one thing: The magnetic field will induce so much current in the bond wires of the chip that it probably will not work to the specs anymore.

Now, in another experiment, we again use a board like the above. The wires are again connected to the far ends. But this time we make a 8cm cut parallel to the longer sides (ok, was obvious, as we cannot make a 8cm cut into a 2cm space). What is the effect now? Independent of the current and the frequency, but as long as the cut is really relatively narrow, we can neglect it's effect. The width of the current carrying path is not significantly reduced and the negative effects of above do not happen.

The lesson we learn is: If you must make cuts into any plane, make them parallel to the current that is flowing through it. This said, we can layout the board right now. Really?

No, no, no! Our simple example can be solved by this, but not a board in the real world. Real boards have many sources and sinks of many different currents. You must know at least the major ones. Then take care that any wire in the ground plane does not narrow the path of any of them significantly. But avoid to force currents in the ground plane to go over the same bottleneck when these currents are not "compatible" to each other. This means, do not force a ground return of an analog signal to go over the same bottleneck with a high frequency digital one, for example. Read the section on the electrical effect further down for an explanation.

Remember, each wire in the ground plane is a cut in it. Keep these cuts out of areas of high currents and if they must be there, make them as much parallel to the flow of the current(s). Better choose another trace to be routed on the ground plane that can satisfy one or both of the conditions. Even half a dozen of traces running parallel to the paths of the currents are better than one running perpendicular and right in a high current region. The last resort is change the layout in such a way that only currents with the lowest frequencies are affected by this cut. So, route DC lines as long as you can and high frequency ones as short as possible. Place any filters or regulators as close to the part where the power or signal is consumed.

And a last remark for those who are not so familiar with microwave design: The mentioned "hot spot" is a very good antenna. Your EMC test lab likes them. Like a dual beacon beam it has two beams that are emitted from your board. Depending on the pieces of your housing where they are reflected they emit at varying slits and openings. You reorientate something in your cabinet - a flat cable or a little metal piece - and your device meets the criteria now, but not then, but again after some modifications. Then fails again. And you do not know where to look for the real source. You suspect the flat cable (but you know it carries only low speed signals and half of the wires are grounded, anyway). Yes, the orientation of the cable produces or suppresses the negative effect. But it does this by reflecting the beam emitted from the hot spot.

The electrical effect.

This effect is very similar to the magnetic, but the details differ. While in the above description the currents created magnetic fields only, they have another property: They produce a voltage loss on any non-superconductive material. Although this can be made pretty small by choosing a thicker ground plane, they cannot be avoided altogether. On raw power supply lines this may never pose a problem. But probably in all other cases. Take a board with the dimensions of the board from above. Again we make a 1cm cut in the ground plane. But this time we run two wires on the other side along the long sides. We connect a DC source to one of the wires and the ground plane and an AC source to the other wire and the ground plane. On the other end we connect a scope at the DC output and a load at the AC output. So, both signals share the ground plane. Moreover we place the two wires really far apart to minimize any coupling between them.

What do you expect to see on the scope? A clean DC signal? Increase the current to the AC load and you will see a proportional bigger AC signal on the DC. (Exchange the scope and the load and increase the DC current and you will see a baseline shift of the AC proportional to the DC current to the load - a proof that it is not a magnetic coupling between the wires.) What then is responsible for the effect? The common series resistor over that both of the signals must flow, formed by the bottleneck. This is not crosstalk. With ICs this is called ground bounce. But it can strike on a board, too. This is the reason, why you should avoid to force "incompatible" ground currents to flow through the same bottleneck. Actually, you should even avoid to run them in parallel, because even the full ground plane has a non-zero resitance.

When you have routed some signals in the ground plane, make a printout of the plane (best is a contour plot, where the copper areas are not filled with ink, but the contours of each wire or structure is plotted only). Identify a source of a major current path, let's say +5V from somewhere on the Vcc-plane. Then pick a major consumer for it, let's say the CPU. Now take a pencil and draw lines that indicate the paths the return current can take. So, start at the CPU ground pins and go back to the point where the power supply connects to ground. (To check your Vcc-plane, too, go further by continuing your line from the +5V from the power supply connection to the Vcc-pins of your CPU. Do this, if you have traces in your power supply plane(s).) Make the line for each path as short as possible. Do not generously make nice slopes around corners - imagine your line would be a rubber band that can move freely within a plane, but never can leave it. (Imagine that the contour lines would be walls that the rubber band cannot flip over.)

After you have identified at least two or three paths your current can flow, mark the shortest two or three ones. Then choose another source of high currents, let's say +12V. And another sink, let's say the output power stage. Again, identify at least two to three possible paths. Mark the shortest ones, but with a different color than the shortest of above. Go on until you have identified and colored the major sources and sinks. When there are more than one major sink for one source, do the procedure for all the sinks.

After that your plot has a lot of colored lines. Look where two or more of different color concentrate. These are the bottlenecks. Do "incompatible" ones flow through the same bottleneck? No, fine. Yes? Try to push them apart by making slots into the ground plane. Place theses slots in a way to make the path through the bottleneck(s) longer than a path that does not run through them. This will degrade the efficiency of your grounding for that path a little bit, but kills the coupling. But do not "overfragment" your plane. Remember, the different parts of your circuit rely on a common ground. Leave enough interconnecting copper for all the currents you haven't considered. There are plenty of them. Done this, your design should work as expected. The last part of this article is not about ground planes, but rather about some other aspects of grounding.

Guard Traces

Do not forget the counterpart of magnetic coupling - capacitive coupling. Whenever the voltage on one conductor changes in relation to some other, this change will induce a change in the other. The emphasis here voltage change, not current change. And a voltage change not necessarily implies a current change of any significant amount. When you feed a signal into a high impedance input you can have voltage variations of tens of volts, but current changes in the pico-amp order (neglectible for magnetic coupling). To minimize capacitive coupling you have two options. First run the traces as far apart as possible - counteracts the increased density of a modern board. Second, run a ground trace between two traces that would be coupled otherwise. This is the most commonly used method. (Capacitive coupling is stronger the closer and the longer traces run in parallel. Traces running perpendicular to each other have a neglectible coupling in 99.99% of all cases.)

This solution is good for most of the cases, but fails in some. Why? Because the ground trace, also called "guard trace", itself has a varying voltage on it. Again, two main sources can be identified here: Either, the ground trace is rather narrow and carries a significant current. Or it's connection to ground is not as good as it ought to be.

In the first case, the worst, the ground trace induces noise into adjacent traces capacitively (voltage changes along the trace due to the impedance/resistance of the trace) and magnetically (current changes induce currents into adjacent traces, see above). As a remedy change the points where this trace is contacted to the ground plane. Choose points on the plane that do not lie along a major path of currents in the plane. Pick them in a way that they lie on the same potential (statically and dynamically). If this is impossible, usually because your ground plane is "criss crossed" by plenty of currents, connect the ground trace only at one point. It should go to the most silent area of the ground plane. Consider a "feeder" trace that starts at a very quit area of the ground plane and runs to your guard trace. You can, when carefully designed, use this feeder trace to feed more than one guard trace. Connect the different guard traces in a star configuration to the feeder trace and make sure that the different guard traces do not carry much current. This is really the last resort, because it can fire back: when a guard trace really does it's job it will get a significant current induced into it. This current must flow to ground (or the guard would not work at all) and the path to it is via the feeder trace. But this feeder trace has a non-zero impedance. When more than one guard trace is fed by this feeder, it will couple from one guard to the others, due to the common mode nature of this configuration. So, use with caution.

In the second case the guard trace cannot drain the induced currents to ground effectively. When using a feeder trace, the combined length may create an impedance, that is too high. Do not forget that about 2.5cm (1") have an inductance of 1nH, narrower traces even more. Without a feeder trace the "aspect ratio" of the guard trace may be too high. "Aspect ratio" is the ratio of length to width here. Make the trace wider, connect it to the ground plane more often or increase the distance to the traces to be shielded. Be careful when you make more connections to the ground plane that you do not make them on noisy regions of the plane, see above.

Confused? Not surprising. Good grounding always has been a science on it's own. Even in the old days of tube amplifiers for a turntable. The rule then was to connect the chassis to electric ground at the most sensitive input. This was the input from the pickup. But still then a dilemma arose: Should you connect the power ground to that point, too? It depended on your circuit. If there was only one - high impedance - input, yes. If there was at least one low impedance input with high sensitivity, no. Better to create a separate power ground distribution and connect that grid to signal ground at the input point. Very often a series resistor with some tens of ohms was used to keep currents flowing through the path power ground - input ground point - signal ground to a neglectible value.

As a final remark: Start your layout by carefully placing the components. Partition your design in a way that keeps signals local as far as possible, especially those with high current or voltage variations. Bulk these blocks and separate them clearly from each other and the rest of the circuit. Never run traces through the regions of these bulks that belong to another part. Make a detour around these regions. By bulking the critical parts and positioning them on the board carefully you can avoid trouble in the first place. Experience shows, that with that technique you have less critical wires to route.

The last rule of thumb: Never violate the ground plane under a part of the circuit that carries high currents or voltages.

© Paul Elektronik, 1998-2002