Crosscoupling in SMPS PCB layout

Question

I have been reading this application note from National and I have a question about this phrase:

... traces carrying switching currents/voltages must also be kept away from ’quieter’ traces to avoid crosscoupling. ...

How many mils should they be away? Does this distance change with the current or voltage? Does the flow of current, voltage affects 'Quieter' traces?

Answer 1

There is no exact answer for how far is far enough. It is better to understand the mechanisms so that you can decide for yourself how to deal with them. There are two independent mechanisms at work that cause cross coupling.

Capacitive coupling. Adjacent traces have finite capacitance between them. Three things drive coupling from a power trace to a signal trace:

• The capacitance. This is a function of how close the two traces are for how long. Longer and closer spacing causes more capacitance, which causes more coupling.

• The rate of change of the voltage on the driving trace. Faster changes (larger dV/dt) will couple better. Another way of looking at this is that faster changes contain higher frequencies, and the coupling capacitance has lower impedance at these higher frequencies.

• The impedance of the signal trace. The unwanted coupled signal has some finite impedance. This forms a voltage divider with the impedance of the signal trace. The lower the signal trace impedance, the lower the coupling.

Inductive coupling. Current in the power trace causes a circular magnetic field around it. This can induce voltages in nearby parallel traces. Essentially the two parallel traces act like a transformer. Two things drive this coupling:

• The coupling inductance. This is a measure of the transformer effect. Like with capacitive coupling, this effect gets stronger as the two traces are closer for longer. Unlike capacitive coupling, the orientation of the traces matter. This coupling is proportional to the dot product of the trace direction vectors (how parallel the traces are in rough laymen terms). Two traces crossing at right angles won't inductively couple at all.

• The rate of change of the current on the driving case. This is opposite but symmetric to the capacitive case where voltage changes matter.

The impedance of the signal trace does not matter for inductive coupling because it causes a offset voltage in line with the trace. It is a additional voltage source in series with the trace.

So, what to do? It should be obvious that moving the traces apart will help for either type of coupling. To reduce capacitive coupling a separating trace or guard trace can be used. Other things that help are limiting the rate of voltage and current changes, avoiding long runs, avoiding parallel runs, and making the signal nets as low impedance as possible. Whether these are possible, under your control, or reasonable considering other tradeoffs like size and cost, are issues with your specific design you have to decide for yourself.

Answer 2

There's no single number here as an answer (otherwise it would probably be given in the appnote). A lot of this comes from experience and intuition (together often called fingerspitzengefühl). Yes, the distance changes with current and voltage. Higher currents create magnetic fields which may induce currents in neighboring traces, and likewise high voltages create electric fields which may induce voltages in neighboring traces. The most vulnerable are traces parallel to and close by the voltage/current carrying trace. So further apart is better, as is shorter length. Also low impedance traces are less susceptible.
Depending on the mentioned factors and how much space you have I would recommend to keep at least 5mm (200 mils) space between the SMPS and the rest of the circuit. If possible surround the SMPS with a ground plane.
Also provide a local ground plane on the copper side under the SMPS, and don't place any components there. (It's worth it to make your PCB double sided especially for this).