label: PCB grounding,printed circuit board
In Part 1: Principles of Current Flow, we began with the basics. We learned that high-frequency signals flow not in the path of least resistance, but in the path of least impedance. We also discussed some fundamental principles of current flow in PCBs with ground planes.
In Part 2: Design to Minimize Signal-Path Crosstalk, we applied those principles to real-world circuits and to the PCB layout of these circuits. We learned how to place components and route signal traces to minimize problems with crosstalk.
In this final Part 3 we consider the power source currents and how to apply what we have learned to circuits with multiple mixed-signal ICs. We finish with an example where a ground plane cut is useful.
What About the Power?
At the end of Part 2 in our series we decided to eliminate the ground cuts in our example layout because there are no signal return currents that "want" to cross the cuts. We do, however, have to consider the power connections. If both analog and digital power is from the exact same supply, then the source and its return must be on one side of the cut or the other (Figure 1).
In this case all the DC return currents (and frequencies low enough that significant current comes from the supply and not the bypass capacitors) from the other side of the cut must funnel through the narrow ground bridge rather than going straight to the power return connection. This makes their path longer, the resistance that they encounter larger, and thus the voltage drops greater.
This layout is no problem for return ground currents where the pins on the ADC sink the signal current, because these currents return from the ground pins which are both at the bridge. However, currents from ground pins on other components have to take an indirect route. Figure 2 illustrates these currents.
Removing the Cuts
If we remove the cuts, the DC return currents can flow more directly, with lower resistance and thus lower voltage drops. Figure 3 shows the same ground currents but with the cuts removed.
The same thinking can be extended to the situation where there are multiple rails. We just have to remember where the return currents will flow and take the multiple rails into account, just as we have done with the single rail.
Grounding Challenge of Multiple Mixed-Signal ICs
We begin this discussion be referring back to the circuit diagram of a single IC in Part 2 (repeated here as Figure 1 above), where all traces are routed to the proper side. Here the cuts serve no purpose because none of the currents "wants" to cross them.
The problem with cut ground planes becomes more apparent when considering a design with more than one IC requiring both analog and digital grounds. Assume that we have two of the same ADCs discussed above. Figure 4 shows this configuration and how it is not feasible to obtain the desired single point ground.
An immediate reaction to this situation could be to rotate one of the ADCs by 180 degrees, thus merging the two into a single point ground. However, that would put the digital portion of one circuit north of the ICs with the analog section south of the ICs; the arrangement would be flipped for the other circuit. The result would be chaos - a mess of analog and digital signals in each other's way. Even if this could be made to work, it does not solve the problem of three or more chips with both analog and digital grounds.
Fortunately, we can apply the same grounding principles discussed in Parts 1 and 2 of this series for a single mixed-signal IC. We imagine that the cuts are there, or we temporarily insert them if we are imagination challenged. Then we place components and route so that we do not allow traces to cross the cuts.
We may also need to keep ADC1's analog signals from sharing ground paths with ADC2's analog signals. This is usually easy to do, as we will naturally be placing the components for each ADC's circuit closer to it than to its neighbor. Figure 5 shows what this might look like with the signal currents shown as red lines and the AC return currents shown as orange lines.
As with the example of a single mixed-signal IC, none of the currents "wants" to cross the cuts so the cuts can be eliminated.
The same thinking can be extended to more complex situations. In general, it is just a good idea to think about where the current will flow for any signal and how it could interfere with, or be corrupted by, other currents flowing through the same metal. This is enough for most applications.
Sometimes Cuts Can Be Useful
There are situations where various mechanical constraints, such as the desired locations of connectors, make it difficult to keep current flow, particularly low-frequency or DC currents, away from circuits that we want to protect. In these cases we may have to resort to judiciously placing cuts in the ground plane.
The desire to avoid such complications is good motivation for considering mechanical placement of connectors along with PCB component placement and routing early in a project. If connectors are placed with consideration for the layout at the outset of a design, it can make the final layout much easier, cleaner, and most importantly, successful.
Even when we carefully consider the interaction between mechanical placements and signal flow, we can easily have situations where external requirements force us to put interfaces in places that make it hard to keep some currents from going where we do not want them to go.
Figure 6 shows a board with digital, analog, and power interfaces in specific locations because of system requirements. We did a good job of placing the noisy digital content adjacent to, but separate from, our sensitive analog circuitry. As noted above, any chips that are both analog and digital are judiciously placed in the bordering area.
We have even done a good job of positioning the power regulators so that the higher-frequency ground returns for analog and digital will not tend to share paths. However, remember that DC and low-frequency power currents will all return to the power source ground which is in the lower left corner by the path of least resistance: a straight line.
The result is that large DC and low-frequency currents from the lower right region of the digital section will run straight through the sensitive analog circuitry. We could fix this by placing a horizontal cut between the analog and digital circuit sections that extends to the right edge of the board. However, we would not want to run the interface signals between the digital to the analog sections across this cut. Routing these traces around the cut would cause them to take a long, indirect route which could be quite impractical, especially if there are a lot of them or if they are particularly fast.
Another idea would be to place a vertical cut between the analog circuitry and the analog regulators, forcing the digital power return current to flow away from the analog circuitry. This would also require us to route the analog power around the cut. Figure7 shows how this would be done.
The DC path of least resistance from the digital circuitry to the power source ground is now no longer a straight line. It is, instead, a path that passes above the cut, thus bypassing the analog circuitry (in all its pristine majesty). This arrangement might be adequate. However it can also be cumbersome if there are several analog supply rails as shown.
In some cases the analog regulators themselves are sensitive with low noise necessary for proper operation of the analog circuitry. Figure 8 shows a different arrangement. The concept is the same as for Figure 7, except that the analog regulators are on the same side of the cut as the analog circuitry.
Sometimes there will be noisy switching regulators followed by filtering and low-noise linear regulators for the analog circuitry. Similar thinking is employed to decide where the noisy switching regulators are placed, always considering where the currents will flow.
Another situation that board-level designers increasingly encounter is the signal integrity of high-frequency signals. As frequencies get higher into the GHz range, we find crosstalk between traces that run close and parallel to each other. This makes things more complicated.
As we have learned earlier, in the simple case of a single trace over a ground plane and as seen in Dr. Archambeault's simulation for 1MHz signals, Figure 12 from part 1 of this series, the return currents are not contained within the area directly under the signal traces but are much wider. It is easy to see how close parallel traces will have their return currents comingle. As the frequencies increase and the traces become a more significant percentage of a wavelength, the signals are more likely to corrupt each other.1
Conclusion - Pay Attention to Where the Current Flows
Many problems with mixed-signal PCB design can be avoided by following this simple advice: pay attention to where the current flows. For most cases all we have to do is remember two basic principles: DC and low frequencies flow mostly in the straight-line path of least resistance between source and load; and high-frequency signals follow the path of least impedance, which is directly under the signal trace. In-between frequencies flow by both paths and in between the two paths.
The idea of using cuts to prevent interaction between different circuits is most often unnecessary, as long as we wisely place components and route traces to prevent this from happening. Sometimes a ground plane cut is needed because we are not always free to choose where components are placed. Again, place the cut wisely, considering all the current flows. We also must remember that no signal should ever cross a cut on any layer.
Keep track of where those pesky electrons want to flow and you will make your job a lot easier. Finally, remember that, "while you can always trust your mother, you should never trust your 'ground.'"
