Printed Circuit Board Design and Layout Questions

1. What are the primary design guidelines that must be followed when laying out a printed circuit board?

In the 10th week of the "Grounding & Shielding" class at Clemson University, students are given a less than optimal printed circuit layout and a list of EMC design guidelines. They are asked to re-layout the board in order to make it comply with FCC and CISPR radiated emissions requirements. At this point in the course, the students have studied crosstalk, parasitics, and basic antenna theory. The design guidelines have been discussed in detail, so the students are fully aware of the reasons for each guideline and how to implement it correctly. Nevertheless, invariably nearly every student turns in a new layout that is worse than the original layout. In many cases, the new designs are even worse than you would expect to get from a board designer who knew nothing about EMC or EMC design guidelines.

How can this happen? I must admit that I was extremely disappointed and discouraged the first time I observed this. However, eventually I came to realize that the problem was not that the students were ignoring the guidelines. On the contrary, the problem was caused by the student's attempt to comply with as many guidelines as possible!

In any realistically complex board design, it's generally not possible to comply with every EMC guideline on the list. The natural inclination of most students (and engineers) is to try to comply with as many design guidelines as possible. This approach, which gives an equal weight to all guidelines is a recipe for disaster. All of the guidelines are not equally important. In fact, there are probably no more than a few guidelines that are critically important for any given design. Unfortunately, the guidelines that are critical will vary from one design to the next, so it is not possible to strictly prioritize guidelines without viewing them in the context of a specific design specification.

What is important, is to recognize the consequences of violating each guideline for your specific design. If violating a guideline causes a specific well defined problem in your design, don't do it! If you are reasonably certain that a particular guideline is not critical in your particular design (most won't be), don't go to great lengths to implement it.

For those who feel lost without design guidelines, there are a few that are nearly always worth considering. A significant percentage of the EMC failures that we have observed in our lab have been the direct result of violations of one of these 4 basic guidelines:

1. Control Signal Current Paths
   Be sure you know how the currents associated with all your signals are getting from the source to the termination AND from the termination back to the source.

2. Control Digital Signal Transition Times
   There is rarely a good reason for the rise and fall times of a digital signal to be shorter than 20% of the bit width. If you are seeing radiated emissions or crosstalk problems above the 10th harmonic of your clock frequency, there is a good chance that your transition times are too fast.

3. Don't Place Connectors on Opposite Sides of a Board
   You should never place high-frequency circuitry between two connectors, because the cables attached to these connectors can be efficiently driven by a few millivolts of noise. When connectors are on opposite sides of a board, there is no good place to locate high-frequency circuitry.

4. Don't Gap or Moat the Digital Ground Plane on a Circuit Board
   Despite what you may have heard, gapping ground plane is almost always a bad idea. Effective power bus noise isolation can be obtained by gapping and filtering the power plane. Analog and digital components can be isolated by component placement and/or returning critical currents on a separate conductor. Attempts to improve EMC or signal integrity by gapping or isolating "grounds" is probably the single most common source of EMC problems on the boards we see in our lab.

References

[1] T. H. Hubing and T. P. Van Doren, "Designing for EMC: The Top 4 Guidelines," Printed Circuit Design & Manufacture, vol. 20, no. 6, June 2003, pp. 22-47.

[2] T. Hubing, "PCB EMC Design Guidelines: A Brief Annotated List," Proc. of the 2003 IEEE International Symposium on Electromagnetic Compatibility, Boston, MA, August 2003, pp. 34-36.