Most conducted EMI problems are due to common mode noise. Furthermore, most common-mode noise issues are caused by parasitic capacitances in the power supply.
For Part I of this discussion, let’s focus on what happens when the parasitic capacitance couples directly to the input wires to the power supply.
1. It only takes a few fF of stray capacitance to fail an EMI scan. Switching powers supplies, by their nature, have nodes with high dV/dt. Mixing parasitic capacitance with high dV/dt creates EMI problems. When the other end of the parasitic capacitance is tied to the input of your supply, a small amount of current is pumped directly onto the power lines.
2. Visualize the parasitic capacitances in your power supply. We all remember from physics class that capacitance between two conductors is proportional to the surface area of the conductors and inversely proportional to the distance between them. Look at each node in your circuit and pay close attention to the nodes with high dV/dt. Think about how much surface area is on that node in your layout and how far it is from the input lines to your board. The drains of switching MOSFETs and snubber circuits are common offenders.
3. Decreasing surface area can be tricky. Try to use surface mount packages as much as possible. A FET in a TO-220 package standing vertically has a huge amount of surface area from the drain tab, which unfortunately, usually happens to be the node with the highest dV/dt. Try using surface mount DPAK or D2PAK FETs instead. By running a primary ground plane on the bottom PCB layer under the tab of the DPAK, the bottom side of the FET is well shielded and the parasitic capacitance is greatly reduced.
Sometimes surface area is needed for heat sinking purposes. If you must use a TO-220 style FET with a heat sink, try tying the heat sink to primary ground (not earth ground). This will help shield the FET and cut down on the stray capacitance
4. Put some distance between your switching nodes and input connections. See Figure 1 for an example of a design where I neglected to follow this simple rule.
Figure 1. Routing the input connections too close to nodes with high dV/dt can increase conducted EMI.
By simply relaying out the board (no circuit changes), I reduced the noise by about 6dB. See Figures 2 and 3 for the measurement results. In some cases, routing the input wires near high dV/dt can even defeat your common mode choke (CMC).
Figure 2. EMI scan from board layout where the AC input and switching circuitry are close together.
Figure 3. EMI scan from board layout where more distance was provided between the AC input and switching circuitry.
Have you been frustrated because after massively beefing up your input filter, you see little or no improvement in the EMI? This is likely because there is some stray capacitance from a node with high dV/dt coupling straight to your input lines, effectively bypassing your CMC. To test this theory, temporarily short out the windings of the CMC on your PCB, and place a second CMC in series with the input power wires feeding your board. If you see a big improvement, you need to re-layout your board and pay close attention to placement and routing of your input connections.
In part II of this topic, I’ll talk about parasitic capacitance inside the power transformer. Email subscribe (top right corner of this page) to the blog so you don’t miss it.
Hi Brian, thank you for the help full article.
Beside the fact, that close proximity of circuit parts to each other, increase the coupling capacity as you described it in your paper.
The first layout is an example for a non optimized layout in many ways. I just like to take out some very obvious parts of the layout.
1.) The magnetic coupling: The transformer which is a flyback transformer for that power level, has no stray field belt around the core, to shield the impact of air gap field against the outside. This field is orientated parallel to the main axis of the transformer, in line with the axis of the input filter choke RF1 acting now as a receiver coil for the stray field. The ability of the filter to damp the low frequency (<1MHz) parts of the EMI noise is decreased( visible in the measurements at frequencies below 500kHz, there seems to be no filter efficiency).
- Swapping the input coil by 90° versus the orientation of the main stray field in the second version of the layout
improves the filter again. A short circuit winding around the filter coil in top and bottom layout, connected to the output of the coil also could further improve the performance.
2.) The electromagnetic parasitics of parts: The two bulk electrolytic capacitors always act also as parasitic foil wound chokes or as an
u-winding (distance pos to minus of the cap with 1/2 the hight of the cap), standing on the pcb.
Putting them close together, helps to build an inductive coupling path, across the filter L.
3.) The coupling path of ground planes: The bulk capacitors in version 1 are standing very close together on two ground planes ( perhaps connected or not, to each other on the solder side?) one plane for the input cap C2 and one for the bulk capacitor of the circuit, its not an ideal ground plane because of the slot on the top side, bridged by the control circuit also transmitting some noise ( Gate Drive Currents).
The caps are parts of the filter and should be separated by some filter inductance from each other to form a Pi-filter.
The coupling capacity between the cans of those caps and the ground planes and the inductive proximity of those caps decrease the performance of the filter.
This has been improved in the second version of the layout, there is no input ground plane any more and the distance between those "filter "part is increased, the control circuit has only one connection to the ground plane after the filter and in not bridging any gaps.
4.) The noise of the snubber circuit: The diode D2 and the RC combination on top of it obviously form the snubber circuit, to reset the transformer and limit the voltage overshoot of the switch. Inside that circuit we find high di/dt and dv/dt transients, transmitting into the environment.
Having a short circuit winding around that circuit ( connected to pos rail) could decrease the magnetic influence.
Having an additional shield plane on the solder side connected to the "calm" positive rail helps to decrease the capacitive coupling paths. - Keep both far away from ground planes.
All content and materials on this site are provided "as is". TI and its respective suppliers and providers of content make no representations about the suitability of these materials for any purpose and disclaim all warranties and conditions with regard to these materials, including but not limited to all implied warranties and conditions of merchantability, fitness for a particular purpose, title and non-infringement of any third party intellectual property right. No license, either express or implied, by estoppel or otherwise, is granted by TI. Use of the information on this site may require a license from a third party, or a license from TI.
TI is a global semiconductor design and manufacturing company. Innovate with 100,000+ analog ICs andembedded processors, along with software, tools and the industry’s largest sales/support staff.