EMI ISSUE

Question

In my previous designs, I used the product with part number LTM2881IY . However, I noticed that this device emits at certain frequencies. Even though I enabled the low EMI mode and used low ESL capacitors , I could not fully overcome the EMI issue since multiple units were used in the design. 
 In my current design, I am planning to use only one device , but at higher speed . Would it be reasonable to add a board-level shield to reduce EMI? Alternatively, could you recommend an isolated RS485 transceiver with integrated power supply that is optimized for low EMI ?

ericb · Accepted Answer

Hello Emirhankose, 
 Adding a board-level shield is certainly one possible EMI reduction technique. In some situations it is needed/appropriate; however it wouldn't be my first suggestion and would be more of a suggestion of last resort. In most applications I believe it should be possible to achieve a desired EMI compliance with the LTM2881 without needing a board-level shield. With proper design, other customers have achieved passing emissions with multiple modules on a single board. 
 I can give you some general suggestions; however, EMI is really a system-level design issue and the entire design needs to be considered. EZ's public nature doesn't make it an appropriate forum for anything more detailed than general comments. If you need more detailed support, I'd suggest you open a technical support case so that your particular application details can be more freely discussed. EMI is an area where the specific details really can matter! You can open a technical support case here: https://support.analog.com/en-US/technical-support/create-case-techsupport/ 
 When trying to reduce emissions, its important that the mitigation technique is well aligned to the type of emissions. Using a differential filtering technique won't be very effective against a common-mode emission source (and vice versa). In my opinion, many of the challenges with EMI arise from misapplying the filter technique to the issue of concern. I'll try to explain a bit behind what's happing here with the hope that by understanding the background better you can better understand the why behind the guidance in the datasheet - which you should read and follow. Also note that while any type of emissions potentially could cause issues, in my experience, for isolated applications, it is usually the common mode emissions which are most problematic and so I'll be focusing more of my explanation there. 
 Isolated transceivers have two different radiated emissions sources: 
 
 Common mode emissions which are generated by common mode voltages due to the isolator's internal switching actions exciting the effective dipole antenna formed by the two ground/voltage domains which the isolator bridges. 
 Differential emissions from switching edge rates or voltage ripple which excite loop antennas with the currents flowing between the device and decoupling/supply capacitances. 
 
 Imbalances and asymmetries in the isolator's internal driver circuit's switching generates a common mode voltage which appears across the internal capacitance of the isolation transformer. The voltage change across this capacitance generates a current which excites the dipole antenna formed by the two voltage domains on either side of the isolator. The emissions from this dipole can be reduced by either preventing the current from flowing into the antenna by adding a stitching capacitor to shunt the antenna or by reducing the efficiency of the antenna by physically reducing the effective size of one of the dipole arms. 
 Adding a stitching cap connected between the two ground domains provides a preferred path for the common mode current to flow which reduces the current flowing into the antenna and generating emissions. For this capacitor to be effective, it needs to have a low capacitive impedance at the frequencies of interest. The effective series inductance within the capacitor plus the PCB traces (and any internal series inductance) will reduce the effectiveness of the stitching capacitor for higher frequencies. For the frequencies generated by isolated supply within the LTM288x modules, typically one needs a combination of a physical discrete capacitor added to the PCB along with the formation of a stitching capacitor within the PCB structure. The discrete capacitor is effective for lower frequencies and the PCB structure for the higher frequencies. Placement and usage of plenty of vias are needed to minimize the parasitic inductance in series with the stitching capacitor. The physical capacitor needs to be selected first for voltage rating and then from the available options one needs to maximize the capacitance while minimizing ESL. Usually this means selecting a capacitor with the highest self-resonant frequency with the required working voltage rating. 
 The area of the isolated side is minimized to reduce the effective size of the dipole antenna "arm" which detunes the antenna. This is achieved by placing a common-mode series impedance (usually ferrites) within all signals leaving the isolator. The common-mode series impedance partitions the isolated side into a small "hot" area that is connected to the isolator and the larger "quiet" area on the other side of the impedance which will include the long cables connected to the transceiver. When adding the ferrites remember to locate them in a copper-keep away area since any copper underneath the ferrite will form a parasitic capacitor which will short circuit the ferrite and provide a path for the common-mode currents which will radiate. Because this is a common mode phenomenon shorting (or omitting) even one ferrite will completely negate the effectiveness of the filter! 
 The above suggestions affect the emissions transmission path; however, one can also reduce emissions by reducing the source. Reducing the input supply voltage to the isolated supply will reduce the emissions source since this will reduce the common-mode voltage difference being applied to the isolation transformer's capacitance which will in-turn reduce the common-mode current being generated by the isolator. The reduction of the common mode current directly reduces the emissions. Thus for the same design otherwise, the -3 (3.3V) version of the isolator will have lower emissions than the -5 (5V) version. 
 Unlike the common mode emissions discussed above, differential emissions issues are potentially present in all applications and so most general guidance on EMI reduction is applicable here. For example, having small, tight loops by placing low ESL decoupling capacitors right at the supply terminals will help. Note that these ripple currents can excite PCB resonances which will need to be minimized/damped. Lowering the edge rate of the signals will also help - selecting slow slew mode when possible helps here. 
 Eric)

SLA Status	Assignee	Support Status
SLA Closed. Met after 16 hours	AndreaRusso ericb	Open

Popular Forums

Product Forums

Application Forums

Design Center Forums

Highlighted Webinar

Places

Libraries

Upcoming Learning & Events

Challenge Yourself!

What's Brewing

Places

Resources

Visit ContentZone

The Latest Read

New Release

Recent Technical Insights

SLA Information

Products Mentioned

Thread Details

EMI ISSUE

Thread Summary

Before You Switch