There are many “rules” for laying out a printed wiring board (PWB) to minimize generation of EMI from a board. These cover a wide range of issues that are important. Some more than others, but all can be important. But, if you were to ask what the number one item on the hit parade would be, what would you say?
What are the important factors to consider when laying out a PWB?
A common area to consider is bypassing. This was discussed a bit in last month’s blog, specifically as it relates to the selection of the size of the capacitor (and whether you should use more than one for a given application). The conclusions that I hope you came to is that the size isn’t really critical, as long as it is big enough and you don’t need more than one for a given application.
So, what else should we consider?
Filtering? This can be important. Probably the most overlooked point is where the filter is located. As a real estate agent will tell you about choosing a house, the three most important things in real estate are location, location and location. Much the same can be said for filters. The best filter in the world, improperly placed in a product, will do you absolutely no good. So, choose the right kind of filter for an application and place it properly. Is this the number one thing that can cause problems? Nope.
How about component layout? This can impact other matters that will be shown to be very important. You do want to keep “noisy” components away from the edges of boards as these locations are likely to be close to openings in the shield, and proximity to openings can have an adverse effect on the shielding effectiveness of the chassis. But, is the location of components the most important factor? Not unless it impacts the most important factor. Keep reading.
Transmission lines. Anything over about 1/10 wavelength at the frequency of interest is no longer a lumped circuit and must be thought of as a transmission line. And a transmission line, to be efficient, should be terminated in its characteristic impedance. If it isn’t, an undesirable effect from an EMC perspective can be ringing. This can cause emissions that aren’t harmonically related to any signals in the product, but are a function of the signal velocity and the length of the transmission line. These can be “fun” to troubleshoot, and fixing them will require additional parts on the board. But, are these the number one problem? Not quite…
How about “grounding”? I’ve had designers tell me that you can’t meet EMC requirements without a solid earth ground. They’ve been very adamant about this until I ask them how a satellite in geo-synchronous orbit meets EMC requirements far more stringent than their PC. And they don’t have a 22,000 mile long ground strap hanging off them. Now, if we’re talking about “grounding” as a solid connection to a common point or structure in the product, that’s a different subject. I told designers that “grounding” was like voting in Chicago – ground early and ground often. There are a number of tricks in “grounding” on boards that can be quite helpful. But, is this still the number one item that I found to be critical? No, but it’s really high on the list.
Conductors leaving the board? This is a very important topic. Wires leaving a PWB can act as antennas. If you have wires leaving opposite sides of the board, you have what looks to the world like a dipole antenna. You have a signal source in the middle and conductors on either side. That can be very bad. Move your connectors to the same side of the board. If you don’t keep RF off those wires you still have an antenna, but just not as efficient an antenna. Radiated emissions will be reduced. They won’t be eliminated, but you might meet the applicable limit.
The number one item is…
Loop area control. Think about this. What radiates the most on a PWB? Current flowing in loops. And how do we calculate the radiation from a loop? Free space radiation from a small loop can be calculated from the following equation:
E = 131.6*10-16(f2AI)(1/r)sin Ɵ
E is the field strength in V/m
f is the frequency in Hz
A is the loop area in m2
I is the current in A
r is the distance from the loop in m
and Ɵ is the angle from the centerline of the loop
These numbers are nice, but there is one factor that you must remember. Radiation from a loop is directly proportional to the area of the loop. If you can control the loop area, you can control radiation from that loop.
How do you control radiation from a loop? Remember that RF is lazy. It must return to its source (remember Kirchoff’s Current Law – the sum of the currents into a node is 0). You can’t have a point in space that is solely a current source, nor can you have a current sink. It must return to its source. And that current will find its way back to the source via the lowest impedance path it can find. That means the lowest inductance path. And that means the smallest loop. The PWB designer controls that loop.
Another way to look at this, and this is important, is that the signals we are propagating from the source to the load are not so much the movement of electrons, but the propagation of an electromagnetic wave through the dielectric of the PWB. That wave exists between the signal trace and the adjacent reference plane (which may be ground or power, as at high frequency RF it doesn’t matter). We need to provide a continuous path for this wave over the entire distance, and the characteristic impedance of this media must not change for best results.
So, how do you control the loop area or the path for the RF wave? There are a number of rules of thumb that describe this. Some of them are:
- Don’t change layers in the board
- Don’t cross breaks in ground or power planes
- Do route high speed traces adjacent to ground or power planes
- Do route clock traces between power/ground planes in 6 or more layer boards
- Do minimize the spacing between signal and return planes
- Keep traces as short as possible, consistent with other design needs.
All of these tend to minimize loop area. And which one of these is the most important? The one that I would insist not be violated under any circumstances, even if it meant violating others? The second one. Don’t cross breaks in ground or power planes. Current tends to flow on the ground or power plane under the signal trace. This keeps loop area to a minimum. This also provides a transmission line for the electromagnetic wave we are propagating. If the signal trace crosses a break in a plane that return current must find a way around it. That will inevitably result in a large increase in loop area. And, as noted above, field strength is directly related to loop area. Don’t do it.
Oh, and does this only matter if a high speed signal is intentionally on the trace? No, it doesn’t only matter in this case. You might have high speed “noise” riding on that trace that you didn’t intend to have on it, and that “noise” still has to have a return path. Crossing breaks in power or ground planes by any trace is a bad idea.
Remember this – loop area control is probably the most important single item in PWB layout. Other factors are important, but if you ignore loop area control you are asking for trouble. This blog is just a short introduction on the subject of PWB layout, but if you remember to control your loop areas, you will be well ahead of the game.