Characterizing & Troubleshooting Wireless and IoT Self-Generated EMI - AltiumLive 2022

Kenneth Wyatt
|  Created: February 3, 2022  |  Updated: February 23, 2022

It is fairly common to find multiple onboard sources of energy causing EMI on today's portable, mobile, and IoT devices. The EMI from these energy sources can couple and often interfere with the receiver performance of cellular, GPS, and other wireless modules. This presentation describes methods for identifying, characterizing, and reducing the coupling from these energy sources. Design PCBs with a Free Trial of Altium Designer Here: https://www.altium.com/altium-trial-flow

Highlights:

  • Issues that arise with self generated EMI’s for cellular and wireless products
  • Three-step process for troubleshooting self-generated EMI
  • Narrow band versus broadband EMI
  • Best possible board design using proper stack-up and partitioning
  • Importance of path of return conduction currents

Additional Resources:

 

Transcript:

Kenneth Wyatt:
Hi, I'm Kenneth Wyatt, an EMC consultant based in Colorado. Today I'll be discussing how I characterize and troubleshoot self-generated EMI for wireless and IoT products. I'd like to thank Altium for inviting me to AltiumLive 2022 CONNECT. I'll let you read the details on my background. But I've authored or coauthored several books on EMC troubleshooting and test, as well as written many articles on this subject for EDN, Signal Integrity Journal, and Interference Technology. My latest publication was my EMC Troubleshooting Trilogy available through Amazon. Volume two on emissions has a whole chapter on wireless self interference if you'd like to learn more.

Kenneth Wyatt:
So why is self-generated EMI such an issue for wireless and cellular products? Platform or self interference is one of the biggest challenges product designers of wireless or IoT devices face today. For example, Apple has dozens of desense engineers on staff to mitigate the myriad of wireless device self interference to receiver modules. The top three sources of the self-generated EMI include system clocks, DC-DC converters, and digital bus noise, with DC-DC converters usually being the dominant source. Many companies incorporate cellular LTE in their products. Cellular providers require a certain receiver sensitivity called total isotropic sensitivity or TIS before a product is allowed on their system. Onboard self-generated EMI can couple into sensitive receivers and decrease the sensitivity to where the TIS test fails. The minimum TIS is about minus 99 dBm, and is also dependent on antenna efficiency. I added a couple links for more information on this test.

Kenneth Wyatt:
There are four possible coupling paths for wireless or IoT devices: radiated from cables, conducted through wires or traces, and capacitive and inductive, which are usually parasitic couplings. Here's a different diagram indicating all four of these coupling paths. Since most portable wireless products will lack cables, the last three couplings conducted, capacitive, and inductive are typically internal to the PC board. We'll be looking at PC board design in much more detail.

Kenneth Wyatt:
Over the years, I've developed a simple three-step process for troubleshooting self-generated EMI. While originally developed to evaluate radiated emissions, the same technique can be used to help characterize self-generated EMI. Step one is to use near field probes to identify high harmonic energy sources on the PC board, and to record the emission characteristics. Step two is to use an RF current probe to measure system cable currents if used. Cables are well known to act as transmitting antennas and radiate harmonic energy. We record the same emission characteristics. Step three is to use a nearby antenna to determine actual harmonic energy being radiated from the PC board or cables. I usually look from 10 to 1500 megahertz initially to observe anything in the usual cellular or GPS bands. We'll look briefly at each of these steps.

Kenneth Wyatt:
Step one is to use a medium sized H-Field probe to identify the major energy sources and to capture their harmonic characteristics. When characterizing self interference, I like to start off by looking from 10 to 1500 megahertz in order to get the big picture. Probing with a near field probe will reveal which energy sources on the board could be producing EMI out into the wireless GPS and cellular bands. In the example, we see a combination of narrow band Ethernet clock harmonics, along with broadband EMI from a DC-DC converter.

Kenneth Wyatt:
Generally you'll see two forms of EMI; narrow band and broadband. Narrow band EMI is represented by a series of harmonically related narrow spikes and is largely due to system clocks, in this case generated by the Ethernet clock. Broadband EMI appears more as an increase in overall noise floor, and is really comprised of a series of such closely spaced switching harmonics that they appear smeared together with is a few broad resonant peaks. When using the typical 120 kilohertz resolution bandwidth as specified by the measurement standard, broadband EMI is typically generated by data bus activity or DC-DC converters. And I find these to usually be the dominant source of receiver interference.

Kenneth Wyatt:
Next, I'll zero in on a specific cellular receiver downlink band, in this case AT&T's band 5 from 840 to 860 megahertz. The yellow trace is a system noise floor, with the aqua and violet traces two DC-DC converters being measured. One converter is 25 dB above the noise floor, and from experience, if this was to couple to the cellular receiver, it would fail the TIS sensitivity test. Step two involves measuring any coupled high frequency harmonic current on cables using RF current probe. If your IoT device includes IO or power cables, these can easily radiate harmonic fields directly into antennas. I'm looking at the same broad or narrow frequency bands as when near field probing.

Kenneth Wyatt:
Once you've characterized the potential emissions from near field and current probing, step three involves using simple close-spaced antennas to confirm whether harmonic fields are radiating or not. You may need to position the antenna very close to observe weaker harmonics. And I'll show an example of this in the case study you later. Kent Electronics is one supplier of simple and low cost PC board broadband antennas. In the link, you'll find an article on how to fashion a PVC adapter to attach the antenna to a tabletop tripod. In measuring countless wireless devices, I've found self-generated EMI is largely due to DC-DC converters. Most of today's DC-DC converter circuits can produce a relatively high amount of broadband EMI.

Kenneth Wyatt:
So why are DC to DC converters so noisy? While the switching frequency of these converters is fairly low, being in the one to three megahertz range, their rise times are in the nanosecond range and can create EMI well above 1.5 gigahertz. If these circuits are located too close to, or are coupling to RF modules or antennas, this can affect received performance. In this example, we'll take a look at a typical buck converter. When S1 is closed and S2 open, AC current flows in the red loop. When S1 is open and S2 closed, AC current flows in the blue loop. Notice that the green loop comprised of the input capacitor and the two switches has AC current flowing for each cycle. Therefore, we need to minimize this loop area to limit EMI, or this loop will radiate like an antenna.

Kenneth Wyatt:
In the example layout on the right, the "hot" loop shown in green is reduced in size and area. This is a good layout. One technique I use to characterize the EMI properties of DC-DC converters is to measure each switched inductor with a medium size H-Field probe. The advantage of this is that measurements may be made without potentially shorting circuitry with an oscilloscope probe. I call this non-invasive probing. The proper orientation for the probe for best coupling is to lay it flat down on each switching inductor, this will couple the most flux lines.

Kenneth Wyatt:
Referring to the schematic, we're interested in measuring the voltage waveform VL across the inductor L. There will be an unknown coupled mutual inductance M between the switched inductor and the H-Field probe. We know the current IL across the inductor is shown in the top equation, 1/L integral VL dt. Vout at the probe port will equal M times the derivative of IL or M divided by L times VL. That is, Vout is proportional to VL, the inductor voltage. Using this fact, we can record all the important EMI characteristics of the switched waveform as we'll see in the next slide. The bandwidth of the probe is sufficient to not affect the measured values.

Kenneth Wyatt:
Here we see the comparison between probing with the H-field probe on the top trace versus probing with a high frequency active of oscilloscope probe on the bottom trace, that's connected directly to the switch node. Other than the pulse amplitude, all other EMI related characteristics are identical. That is the rise time, pulse width, period, and ring frequency. The two most important EMI measurements are the rise and fall times, and the ring frequency. Using this non-invasive technique prevents potential missteps using oscilloscope probes, and really speeds up the analysis and characterization of the converters.

Kenneth Wyatt:
It turns out ringing has quite an effect on the emission spectrum. This occurs often with switched mode power supplies, and will be demonstrated in the next two slides. The ring frequency will produce a matching resonant peak in the emission spectrum for a product. The ringing is due to parasitic inductance and capacitance in the circuitry of the switched mode power supply. This resident peak can often accentuate coupled EMI in the various wireless and cellular LTE bands. Here we're measuring the switched waveform from a one megahertz DC-DC buck converter using a gallium nitride switch device. We're using a Rohde & Schwarz RTE 1104 oscilloscope with a RT-ZS10 1.5 Gigahertz active probe to make the measurement.

Kenneth Wyatt:
You can see the very large ring wave with a frequency of about 217 megahertz. Here's a closeup of that ring frequency along with a resulting emission spectrum. Measuring the power supply input current with a current probe, we see a peak at the ring frequency of 217 megahertz in the aqua trace. Measuring the power supply output current, we see peaks at both the fundamental 217 megahertz and second harmonic of 434 megahertz, as well as higher harmonics extending into their cellular LTE bands. Note the very broad band emission spectrum from the one megahertz switching power supply. This is very characteristic from today's onboard switching converters.

Kenneth Wyatt:
I recently acquired an EMScanner system from Y.T.C. Technologies. The scanner includes an array of tiny H-field loops within the sensor board. Placing a PC board on the array will plot a heat map of the electromagnetic fields. I'm starting to use this to help evaluate the fields around the board and attached cables. Results look promising so far and is an additional troubleshooting tool to help map out hotspots on wireless boards. So knowing that DC-DC converters used on today's embedded processors are a dominant source of potential interference to sensitive onboard receivers, let's look at the top 10 ways to reduce DC-DC converter EMI.

Kenneth Wyatt:
Tip one, get the PC board stack-up correct. There are two very important rules for good PC board design and most commonly used designs from decades ago failed to follow these. Above 100 kilohertz all signal and power transients propagate as electromagnetic waves within the dielectric space between the trace and return plane. Rule number one is that all signal traces and power planes or traces must have an adjacent solid return plane in order to bound the electromagnetic wave. Rule number two is that all power planes or traces must have an adjacent solid return plane in order to bound any transient electromagnetic waves. A third point is to make sure all critical signals have a defined return path back to the source. A good example is when running signals from top to bottom on the board. Note for critical mixed signal and wireless designs, this precludes using the power plane as a return path, except in limited situations. These rules will dictate the stack-up design. For more details, see the linked articles in the references.

Kenneth Wyatt:
First let's review the path of return conduction currents as this is the key reason partitioning of circuit functions is so important. Here's a simulation of this concept with a return conduction current in green. For the low frequency one kilohertz example on the left, we see the return current is spread out and basically travels from the load directly back to the source, the so-called path of least resistance. In the high frequency one megahertz example on the right, we see the return current located directly underneath the circuit trace, or the path of least impedance. Most onboard DC-DC converters are now operating at one megahertz and above, so return currents will tend to follow right underneath signal traces. Because return currents are largely confined under the signal and power traces above 100 kilohertz, we can use the concept of partitioning to isolate various portions of the circuitry. This concept of partitioning will be very important when we loud our circuit board between analog RF and digital circuitry. I'll show a slide that later describes this better.

Kenneth Wyatt:
There are two viewpoints when it comes to how signals move in PC boards, the circuits point of view and the fields point of view. In reality, they are related. That is, you can't have one without the other. Now the circuit theory point of view considers only that signals and power sources return back to their sources, and this was hammered into us as undergraduates. To fully understand low EMI PC board design, requires we also consider how the signal energy in the form of electromagnetic waves propagates in circuit boards. When considering the fields point of view, we need to understand that signal and power transient fields travel in a dielectric space at near light speed, while the conduction and displacement currents simultaneously flow back to the source along the inside surfaces of the copper traces and return plane at about one millimeter per second. The important point is that the signal energy is in the fields, not the copper.

Kenneth Wyatt:
So how do digital signals propagate in a simple microstrip? Let's assume a microstrip over a solid return plane is pictured in the cross section. On the left we have a gate driver and on the right a resistive load at the characteristic impedance of the transmission line. Above 100 kilohertz, the digital signal is actually an electromagnetic wave traveling within the dielectric space between the copper trace and the return plane with a Wavefront propagating from left to right as the gate goes from a high to low state in this example. It is important to note that signal propagation is not through to the flow of electrons in copper as has been long implied. The electromagnetic wave induces a conduction and displacement current, which does flow along the inside surfaces of the copper trace and plane and through the dielectric as displacement current, respectively, but at a very slow speed of about one millimeter per second. This conduction current is what you'd measure with an ammeter.

Kenneth Wyatt:
For FR4 dielectric, the wave propagates at about half light speed or about six inches per nanosecond. Most four layer boards I review uses very common but very high EMI risk stack-up as shown.The first thing to note is that the power and return planes are too far separated for good high frequency decoupling, thus you'd expect to see power transients being radiated. For best high frequency decoupling, the power and return layer should be no more than two to three mills apart. The second point to note is that there is a signal layer referenced to power plane, return conduction currents want to flow back to the source, which is usually reference to the return plane not power. It's possible to reference signals to the power plane for noncritical circuits, if and only if the power and return planes are very closely coupled together, and with adequate decoupling capacitors. However, for the classic four layer stack-up, this is hardly ever the case.

Kenneth Wyatt:
There are probably many solutions to the typical four-layer conundrum, but here's a couple that will work well for you to achieve lowest EMI. In each, we're running signals and routed power on one layer, and the only difference is whether the ground reference planes are on the inner or outer layers. The advantage in running the signals and power on an outer layer is that they are easier to get at for troubleshooting. On the other hand, the advantage of positioning the reference planes on the outer layers is that they can be stitched around the edge to provide a Faraday Cage effect for better board self shielding.

Kenneth Wyatt:
The disadvantage for both is that you'll need adequate decoupling capacitors at each power and return pin for critical ICs. For really small and dense designs, it's usually best to use 8 or a 10 layer board stack-ups to begin with. The most commonly used six-layer stack-up shown on the left has similar issues. The first thing to note is that the power and return planes are too far separated for good high frequency decoupling, thus you'd expect to see power transients being radiated. Not only that, and more importantly, power rail transients will couple to the two signal layers, three and four.

Kenneth Wyatt:
For best high frequency decoupling, the power and return plane should be no more than two to three mills apart. Closer is even better. Again, the second point to note is that there is a signal layer reference to the power plane as discussed previously. The suggested stack up on the right follows the basic rules of trans mission lines, and also allows the power and return layers in the middle to be more closely spaced for better high frequency decoupling. Disadvantages include losing one signal layer; however, for today's high density wireless products you'll likely require 8 or 10 layers anyway for best circuit performance and lowest EMI.

Kenneth Wyatt:
Because return currents tend to flow directly underneath signal and power traces at frequencies above 100 kilohertz, we can use this self-isolation property to separate noisy circuits from quiet circuits through the use of partitioning of major circuit functions, and yet use a solid return plane for the board. For example, by keeping the digital processing separate from the RF sections, we keep the associated noise return currents from coupling to sensitive receivers. While I indicate power distribution by a blue line, in reality you should generally use is a solid power plane for the primary 3.3 volt digital source, and can optionally run it across the entire board depending on the power requirements of the system. It should certainly be a solid power plane under all digital processing circuitry and using plenty of decoupling capacitors to the return plane.

Kenneth Wyatt:
It's not always realistic to separate circuit functions in the simplistic model shown, but it is very important to isolate known noise sources from wireless and cellular modules. Grouping all the wireless circuitry together and away from noisy digital processing and power converters is a key goal. And while I show the power conversion as a separate block, it is often located closer to the power input connector OR also distributed closer to the load it's powering. I'd still keep all DC-DC converters far away from wireless modules.

Kenneth Wyatt:
Tip two, use low EMI converters. Both Texas Instruments and Analog Devices or Linear Technologies continue to develop low EMI converters, and I'm sure other manufacturers are doing the same. For example, TI has developed new QFN packaging that allows the input and output capacitors to be located closer to the package. Some of their devices also include means to control the slew rate of the switched drive voltage. Analog Devices has developed their silent switcher, which also accommodates locating the input and output capacitors, particularly close to the IC package. Their newer Silent Switcher 2 low EMI converters incorporate both the input and output capacitors and their associated loops within the IC package. And finally, their micro module design also incorporates the switching inductor as well. While more expensive, these are all particularly quiet for EMI in wireless applications. Finally, many converters have an option to use spread spectrum clocking, which can further reduce the average EMI.

Kenneth Wyatt:
Tip three, keep converter circuitry on the same layer. One issue that creates noise coupling is running fast switching signals from the top to bottom of the PC board. I had a one client locate the buck converter circuitry on the top layer and the output switching inductor on the bottom layer of their board. The resulting three megahertz switching currents flowing from top to bottom and back created enough interference to block onboard GPS perception.

Kenneth Wyatt:
Tip four, keep converter circuitry close to the IC. We already mentioned DC-DC converters always have an input current loop and an output current loop as shown, these loop areas must be minimized. IC manufacturers are starting to recognize EMI is an issue and warn designers about this. The converter manufacturers often towards the end of the data sheet, offer a suggested layout. Layout suggestions even in the last two to three years are often inaccurate, if older than that are usually incorrect. Both the input and output capacitors along with the output inductor should be located as close to the IC packages possible to minimize these loops. Another important point is to avoid intermixing the input and output circuitry of converters on the board layout. We want to keep the primary and secondary circuits as separated as possible. Finally, don't allow the input and output capacitors to share the same return current path.

Kenneth Wyatt:
My colleague, Dr. Todd Hubing of www.learnemc.com has excellent presentations on laying out DC-DC converters. See the references for a link to his site. Tip number five, the ground return plane must be solid. Fast switching signals or converter traces crossing gaps or slots within the ground return plane, will couple EMI throughout the board and can couple into sensitive receivers. I have a short video demo on my website explaining why gaps in the return plane are a disaster for EMI. You can see the difference in emissions for a gap versus ungapped return plane in the right hand screen capture.

Kenneth Wyatt:
There's about a 15 to 20 dB increase in EMI if return currents are forced around a gap in the return path. There's been an ongoing debate on whether it's best to place voids in the return plane under either the switch node, the switch inductor, voids under both, or keep a solid return plane. Steve Sandler of Picotest created a set of buck converter circuit boards with each configuration, and I measured them a number of different ways, with a current probe on the power input or using a LISN with the ability to extract just the common mode or differential mode EMI. In each measurement, the solid plane came out the overall winner at most frequencies, at least within measurement error. In most cases, the differences were slight, just 2 to 3 dB, but this could still mean complying or not if you are right on the edge.

Kenneth Wyatt:
Tip number six, the switching or output inductor should be shielded, this helps confine the magnetic fields. In the cross section shown on the left, we can see the winding on the left half is covered with additional ferrite, and the magnetic fields are bound to just within the gap areas. On the right hand cross-section, the field lines are unshielded and are free to radiate and couple to other circuits. In the plots and simulations by Patrick DeRoy, you can see quite a difference. Basically, if you can see the windings, it is not shielded. Here's another plot from Patrick DeRoy showing the difference in magnetic field between the shielded and unshielded inductors. And there's about a 15 to 20 dB difference.

Kenneth Wyatt:
Tip number seven, orient the output inductor for low EMI. Here's a trick that most aren't aware of, inductors have a start and an end on their winding. The start terminal is sometimes marked on the top of the body with a half-moon, dot, or a line. For example, Würth Elektronik tends to use a line or a dot. TDK uses a half moon. Because the start of the winding is buried by the total turns, it is somewhat shielded by those same turns. Orient the start of the winding so it can to the switched node often labeled SW of the DC- DC converter IC. The end of the winding connects to the output filter, so it's going to be quieter or more filtered than the start of the winding. This could potentially reduce the EMI by 2 to 3 dB, according to PC board expert, Rick Hartley.

Kenneth Wyatt:
Tip number eight, plan for local shields. Despite the use of ally shielding inductors, good PC board design and layout practices, there will still be strong H and especially E-fields generated around the circuit loops and output inductor. Design your PC boards to accommodate these local shields right from the start by adding fencing solder strips connected to the ground return plane. You may also need to add these around the processor and memory Ics, and if you don't need them then great. Würth Elektronik, Layad, and many other manufacturers make these standard and custom local shields. I found by experience, it's very difficult to tack solder temporary shields if these solder strips are not designed in at the start.

Kenneth Wyatt:
Here's another measurement by Patrick DeRoy showing the reduction in E-field and H-field by using a local shield one centimeter above the PC board. You can see a rather dramatic reduction in E-field on the left, which if not shielded could radiate directly into wireless antennas. This shows the results of a study on the use of local shields by engineers from Samsung. Note the almost complete lack of fields in the shielded phone on the right. Most mobile phones today use multiple local shields over most of the circuitry

Kenneth Wyatt:
Tip number nine, use RF absorber. One promising mitigation is flexible ferrite loaded RF absorber. I've amassed quite a collection through the years, but early experiments seem to offer little help at cellular frequencies. I'm going to dwell on this tip for a few slides, because I believe there is a real opportunity to reduce internal couplings to receiver modules, and I'd like to encourage others to experiment with this material. Würth Elektronik published an application note ANP059, that described three methods for characterizing this RF absorber depending on the application. The one that would be most useful for absorbing electromagnetic fields was the microstrip method as described in the slide. The technique simply measures the attenuation through a microstrip when the ferrite material is laid over the top. Attaching the absorber to devices or traces with high frequency harmonic content helps suppress any radiating fields

Kenneth Wyatt:
Because most manufacturers don't seem to provide the sort of absorption data I required, I set up a scaler network analyzer and started characterizing all the samples I had in order to find a material that was effective in the 600 to 1500 megahertz range. I discovered most of my samples were only effective in the microwave frequencies, but I did find a few that worked in the more common wireless and cellular bands. The testing went very quickly because all I needed to do was position each sample over the 50 ohm microstrip and record the results. The results of this study are mentioned in the references. Two of the best I found for the important wireless and GPS bands were Parker-Chomerics SS4850 0100 0150 300, and Arch Techs WAVE-X WXA20 absorber materials. You can see at least a 10 dB absorption in the cellular LTE band and up to 20 dB in the GPS band for each material.

Kenneth Wyatt:
In this case study, I was assisting the client in reducing cellular desense in several bands. There were numerous energy sources creating self-generated EMI. In this experiment, I attached the self-adhesive Arc Tech WAVE-X WXA20 patches on top of a DDS RAM, a flex cable known to be hot with RF, and a power management IC containing several DC-DC converters. And these are shown by small red "X"s.

Kenneth Wyatt:
In the case of this IOT device, the cellular antennas were located top and bottom with GPS and wifi antennas in the sides. We were getting a strong video signal leaking from the side of the PC board right in middle of the LTE Band 5, which is an AT&T band. Following application of the three small absorber patches, that strong signal dropped by at least 15 dB into the noise floor, and cellular received sensitivity was greatly improved. I believe there's much more opportunity in using ferrite loaded absorber for dealing with high frequency energy sources, such as DC-DC converters. The issue is that most of this material is designed for the microwave bands and is ineffective in the bands used by most IoT devices.

Kenneth Wyatt:
Tip number 10, locate antennas and coax cables away from DC-DC converters and other cables. Antennas and their associated coax cables if used, should be located as far as possible from DC-DC converters, processors, and IO or power cables. As we saw in previous slides, the input circuit loop of large voltage drop buck-verters will have a relatively high dV/dt, and the associated electric field can couple directly into the receiver antenna. In addition, IO and power cables can couple common mode currents generated on the board directly into antennas.

Kenneth Wyatt:
Well, here's a bonus tip number 11, don't trust IC manufacturers' data sheets. While some data sheets are accurate, very often the EMC design and layout advice is just plain wrong. Here are a couple examples from TI. And don't assume TI is the only one providing incorrect design information, they all do on occasion. On the left, the TI TPS54308 makes a solid return plane unclear. The switch node runs all over the board and the input and output capacitors share the same ground return path. The switch node needs to be minimized in area and located close to the IC.

Kenneth Wyatt:
On the right, the suggested layout for the TI LMR 33630 also has the input and output capacitors sharing the same ground return path. This is a great way to couple switching voltage directly to the secondary power rail. Dr. Todd Hubing presented an excellent paper on just this topic regarding manufacturer's data sheets and application notes during the 2020 IEEE Symposium on EMC and SIPI, he also includes this topic in his courses at learnemc.com. So here's a long list of things to try if experiencing self-generated EMI, which is affecting your TIS test of receiver sensitivity. After experiencing dozens of client projects, some of these experiments will help pinpoint issues and some may not. I won't go through the entire list, but would like to demonstrate a couple ways of positively identifying which DC-DC converter or converters are coupling to the receiver

Kenneth Wyatt:
Because most IoT devices use embedded processors requiring three to five power rails, one very useful trick to determine which converters are creating the dominant EMI is to replace them with batteries or tack on 3-terminal linear voltage regulators. Now, this is easier than you might think because it only involves removing the switching inductor from the board and tapping into the power rail. Removing the inductor stops the switching activity. We've used either battery packs with series Schottky diodes to drop to the correct level or soldered in three terminal linear regulators. Once these EMI sources have been identified, then focus can be turned towards that area of the PC board for identifying possible coupling pads

Kenneth Wyatt:
In summary, to achieve the very best receiver TIS performance, we need to ensure the board design is the very best possible using proper stack-up and partitioning. We also need to ensure DC-DC converter circuitry is closely spaced together and on the top layer with solid return plane below. We will very likely require local shields over high energy sources like DC-DC converters, processors, and memory. Try adding RF absorber to known energy sources like radiating traces, processors, RAM, and DC-DC converters. Proper wireless and cellular antenna placement can also be a key factor.

Kenneth Wyatt:
Here are a few resources I've found to be helpful as well as some of my articles that go into more depth. Self-generated EMI has been a long time issue with manufacturers who are developing wireless and cellular IoT products. I hope these tips help you achieve low EMI noise coupling to your wireless and cellular receivers. For more information on troubleshooting wireless EMI issues, or general EMC troubleshooting, you might check out my blogs on design-4-emc.com, or on EDM, or interferencetechnology.com, or my Amazon author page.

About Author

About Author

Kenneth Wyatt is principal consultant of Wyatt Technical Services LLC and served three years as the senior technical editor for Interference Technology magazine from 2016 through 2018. He has worked in the field of EMC engineering for over 30 years with a specialty in EMI troubleshooting and pre-compliance testing. 

He is a co-author of the popular EMC Pocket Guide and RFI Radio Frequency Interference Pocket Guide. He also co-authored the book with Patrick André, EMI Troubleshooting Cookbook for Product Designers, with forward by Henry Ott. He recently completed and released a three-volume “EMC Troubleshooting Trilogy”, which is now available through Amazon. 

He is widely published and authors a monthly column, The EMC Blog, which is hosted by EDN.com and continues to write for Interference Technology and the Signal Integrity Journal. Ken is a senior life member of the IEEE and a longtime member of the EMC Society. To contact Ken or for more information on technical articles, training schedules and links, check out his web site: http://www.emc-seminars.com.

Recent Articles

Back to Home