Design Tips: EMC Effects from the Hidden Schematic
Welcome to this new section of the EMC Newsletter! “Design Tips” will be brought to you in each issue to further your education on the practical side of EMC. There is a lot of very good accumulated knowledge about EMI/EMC design within our community. This new section is intended to help people share this knowledge with everyone else, without the need for submitting a formal paper. The goal is to have a short (1-2 pages) description of different design tips followed by a “real world” example that could be useful to others in the EMC community. But, this means I’ll need your help! Please send me your most useful design tip for consideration in this section. Ideas should not be limited by anything other than your imagination! Please send these submissions to I’ll look forward to receiving many Design Tips! Please also let me know if you have any comments or suggestions for this section, or comments on the Design Tips articles. This first Design Tip concerns one of the most misunderstood concepts within EMI/EMC design….”GROUND”.
Editor’s Note: Many thanks to EMC Board of Directors Member, Elya Joffe, and his Membership Development Task Force Committee, who suggested creating a “Design Tip” section of the Newsletter to enhance member benefits. Thank you too to Dr. Archambeault for his willingness to coordinate these articles as our newest Associate Editor.


Electrical engineers are quite familiar with schematic drawings. While the schematics are accurate for the intended signal flow, there is a very important piece of the signal path missing! The signal voltages are usually all referenced to “ground”, and the schematic assumes that all these signals have a common reference point. However, this is not true for high-speed signals.
The concept of “ground” requires that a large area (PCB or metal chassis, for example) be at the same potential/voltage. At low frequencies (for example in the audio frequency range) this is easily achievable, and the concept of ‘ground’ has definite meaning. However, at today’s high speed data rates, the frequency content of the signals is significantly higher, resulting in wavelengths that are much smaller than the ‘ground’ area we use. This results in a voltage difference across the ‘ground’ plane (or chassis) and makes the concept of ‘ground’ at high frequencies completely meaningless. When dealing with high frequency signals, it is important to remember, “Ground is a place for potatoes and carrots”! There is no magic about ‘ground’…it is simply a possible current path.

The important point is that for EMI/EMC we need to consider the current, not the voltage, in our signal paths. Since current must always flow in a loop back to its source, the return current path must be considered as well as the intended signal path along a PCB trace. Any interruptions to the return current path can have serious negative effects to the EMI/EMC performance of a PCB. A very slight deviation in return current path can result in enough inductance to dramatically increase emissions.

Figure 1. Initial Two Board Configuration
Figure 2. Return Current Paths for Initial Configuration

The return current path is also very important when considering mother/daughter board configurations. Figure 1 shows a simple 4-layer board example of a mother/daughter board configuration and a signal path from the motherboard to the daughter card through a connector. If we consider how the return current will flow from this configuration, we should expect that the return current would spread out to include displacement current through the dielectric between GND and PWR as well as local decoupling capacitors (depending on their distance and the plane separation). Figure 2 shows the return current for this configuration. The added return current path length results in additional inductance in the total path, resulting in a ‘noise’ voltage between the two GND planes (across the connector). This noise voltage will drive the wide, thin, monopole-like antenna, resulting in increased emissions.

Figure 3. Improved Return Current Design

However, if we had simply considered the return current path and routed the signal trace so that it was referenced to the same plane (PWR or GND), the return currents are able to stay close to the signal trace (Figure 3), and emissions are greatly reduced.
When we consider the return current path, more ‘ground’ is not always the ‘right’ answer! For example, on a recent design, there was a 144-pin connector with many high-speed signals traveling from one board to the other. It was determined that 30 pins could be used for ‘power’ and ‘ground’ combined. At least five pins must be ‘power’ so there would not be an excessive DC voltage drop across the connector. How many of the remaining 25 pins should be ‘ground’?
In this particular design, it turned out that about 2/3 of the total signal pins were referenced to the ‘power’ plane, and only 1/3 referenced against the ‘ground’ plane. This meant that of the total 30 possible power/ground pins, 2/3 should be ‘power’ and only 1/3 should be ‘ground’! More ‘ground’ pins was NOT the best design for this case. Of course, once we consider both the ‘power’ and the ‘ground’ pins to be return current paths, it is obvious we should distribute them throughout the signal pins to keep the return current deviation as small as possible (compared to putting all the ‘ground’ pins at the ends of the connector, etc.).
The ‘ground’-to-‘ground’ noise voltage is very real. A simple differential voltage measurement between the ‘ground’ layer on a motherboard to the ‘ground’ layer on a daughter card (in this case a memory DIMM) is shown in Figure 4. A noise voltage of 0.8 volts peak-to-peak was measured for a signal strength of 2.5 volts! Nearly 1/3 of the total signal voltage swing was just ‘ground’ noise. In this example (Figure 4), no consideration was given to the return current path and the resulting noise between ground-references on the two boards was significant.

Figure 4. Measured Example of Ground-to-Ground Noise from Poor Return Current Design

When we consider the most important concerns for good EMI/EMC design, the schematic is not as important as the physical layout of the signal path and the return current. Since today’s high speed PCBs have many layers and are very complex, it is difficult for an engineer to examine each critical signal path for a good return current path. Automated EMC rule checking tools can examine each net in turn, regardless of the PCB complexity. The key to selecting an automated rule checking tool is to make sure it can interface well with your existing design process, it is easy to use, and it can display rule violations in a graphical and easy to understand manner.
The most important EMC design rules for high speed PCBs concern the return current path. Since the return current will always find a path that minimizes the inductance of that path, the return current will always flow on the nearest plane, whether it is called ‘ground’ or ‘power’ or ‘carrots’. When traces cross a split in the return plane (for example, if a trace is routed next to a power layer with multiple power islands), the return current’s path is interrupted. Changing layers within the PCB so that the return current must also change planes will also interrupt the return current path. Remember, the return current must always get back to its source. It will get back to its source. The only question is whether it will be a path that is beneficial to you, or if it will cause problems. So, “Do you feel lucky today?” It is always best to design ‘on purpose’ rather than ‘by luck’. EMC

If you would like to contact the IEEE Webmaster
© Copyright 2006, IEEE. Terms & Conditions. Privacy & Security

return to contents
IEEE logo