Board layout guidelines from National Semi’s Jon Dutra and the mistake of single-point grounding

I got a note last night from my FAE (field application engineer) buddy Jon Dutra. He was helping a customer with some board layout problems. He sent along some general rules he advises people on regarding printed circuit board (PCB). Jon’s notes:

Trace impedance is an RF term , distributed L and C forms a characteristic impedance for a trace or wire. In an audio circuit the trace lengths are short compared to an audio wavelength, even for most switchers the trace lengths are short compared to the wavelength, or periods. I mostly deal with these as "Lumped impedances" ( Capacitance etc) It may be useful to deal with a few traces as controlled impedance, especially outputs, but the rest get the rules of thumb for circuits below 5 MHz. Now there are a few "Rules of thumb for circuits below 5 MHz" …………………………

• The smaller the signal, the smaller you want the node (Microphone inputs are very small signal)
• The higher the node impedance (Z), the smaller you want the node.
• The higher the gain from the node, the smaller you want the node. (By small node I mean narrow, short trace)
• Op amp inputs, especially the negative input, are VERY sensitive nodes, ( high Z and high gain) and should be made as short / small as possible.
• Op amp outputs are low impedance, they can generally be routed "anywhere".
• Solid ground planes are your friend for rejecting RF

Rules of thumb for circuits above 5 MHz", extensions, when frequencies (usually logic) exceed 5 MHz and / or trace lengths are longer than 6 inches.

• Here controlled impedance makes sense.
• I love source termination for 90% of my signal propagation needs.
• You do not need an exact impedance match. I generally put 30 ohms in series with all logic gate outputs if I am at all concerned about EMI on that line, right at the source.
• I generally put 30 OHMS in series with all amplifier outputs (outside the loop) if I am at all concerned about EMI on that line, right at the source.
• Of course that resistance can be modified, down or up, once board is fabbed, but if 30 ohms does not work you have other issues ! (Like race conditions or critical timing or heavy loads).
• Yes 30 ohms is not the trace impedance, no big deal in 99 % of applications.
• The load(s) are generally not terminated, or terminated in 10 K ohms or more.

There are other advantages to source termination as well……….

• Only one resistor.
• It provides great signal swing.
• It provides inherent short circuit protection.
• It isolates the source from complex reactive loads.
• It provides damping on the line.
• It terminates the line for RF circuits. The longest reflection is only twice the line length.
• It low-pass filters the line, reducing EMI.
• And all it costs is a resistor in series with the output.

It is not perfect however ….

• It limits the maximum power from the source, possibly good, possibly bad.
• It slows down any edge, possibly adding jitter.
• But again, if it is a problem, use ten ohms or zero ohms.

There is a lot of good stuff here but I really like Jon’s comment about how a continuous ground plane, with no slots or cuts or divisions into an “analog” side and a “digital” side. In my 20 years of consulting I had always found that having a continuous ground plane was essential, especially in high-speed design. It was only when I heard signal-integrity consultant Henry Ott give a lecture a few years ago did I hear that same sentiment being voiced by people with big-time credentials. Henry used to work at Bell Labs and was in their Long Lines division.

At the DesignCon show this month not a single person on a panel or speaker recommended cutting up the ground (reference) plane. They said it is best to have separate power planes but if you have to cut them up, they tried to give rules. There was one guy in the audience that just did not believe that you should not cut up the ground plane, he had read it in so many app notes. He did not understand the IC designer’s problem of bond-wire impedance– he figured if the chip had an AGND and a DGND that meant he was supposed to have two ground planes.

One of the panelists had my exact experience when I consulted– the more cut up the planes the more money you could make stitching them back together. This does not disparage Jon’s method of top-side pours for switcher ground tied to the real ground at the common of the output cap (see figure 5 and 6 and associated text).

And I pretty much got an entire panel to admit the audio guys are wrong with single-point grounding. I still don’t think they understood fully my point that no circuit is 20kHz. Every single circuit on earth is 1.8GHz since that is the cell phone frequency you have to keep out of your signal path. Sure, doing a full reference-plane ground scheme might make the Audio Precision readout 0.0006% distortion rather than 0.0004%, but then again, you won’t hear zzzzzdt zzzzzdt zzzdddtrtsz every time your cell phone negotiates with the tower. It turns out that this was the exact problem that one of his customers was having that prompted Jon’s note to me. I should also mention how we are seeing more and more systems designed to have the power and ground planes on the outer layers, with all the signals shielded within on the inner layers. That is the problem with single-point ground schemes, it makes many if not all of the ground runs high impedance. As National’s Ed Fong reminded me at lunch yesterday, the wavelength of a propagating signal is divided by the square root of the dielectric constant. So if FR-4 has an e of 4.7 that means the wavelengths are about half as long as in free air. This is shy you only need a centimeter or so of PCB trace to make a dandy antenna that can pick up cell-phone frequencies.

Oh, and Jon mentioned National’s EMI resistant op-amps, the LMV831, 832 and 834.