3
\$\begingroup\$

I have 4 opamps which need +12 V and -12 V supply voltage. I have 2-layer PCB and want to keep it that way; the bottom layer is dedicated for GND of course. To keep noise/EMI as low as possible, +12V and -12V should be routed close to each others to each opamp. But that would mean quite a few passes to bottom layer and back to top layer and breaking GND layer.

So what should I aim at:

  1. Keeping +12 V and -12 V on top layer as much as possible: More solid GND layer but bigger space between them +12 V and -12 V.
  2. Routing +12 V and -12 V as close together as possible: Break GND layer more but smaller space between +12 V and -12 V.
\$\endgroup\$
3
  • \$\begingroup\$ If you use wire jumpers, you can keep the ground plane intact. You'll have both benefits. \$\endgroup\$ Commented Nov 26, 2012 at 2:14
  • \$\begingroup\$ Yamaha can design it with single layer copper and jumpers. OPA1602 or 1604 quad is even nicer. Keep inputs close to shielded jacks. Avoid ground loops. Use good V+- filters on supply close to chip with ferrite beads. \$\endgroup\$ Commented Nov 26, 2012 at 2:52
  • \$\begingroup\$ If you make a two-layer board for audio, and you still need jumpers, that's an epic fail. And lots of pro-audio gear has been built with one-layer boards. \$\endgroup\$
    – Kaz
    Commented Nov 26, 2012 at 2:58

3 Answers 3

4
\$\begingroup\$

Dedicating a layer for grounding is not necessary in audio. Ground planes are an RF technique. At audio frequencies, you're not worried about effects like currents leaking across the epoxy substrate.

I just built a dual-supply (+/- 15V) audio board with four op-amp IC's, like yours.

(It was originally going to be a single layer design with a few jumpers, but then I decided to go with a manufacturer that makes two-sided, so I rerouted it.)

The +/- 15 power rails are strictly in the top copper, and the bottom contains the ground traces (not pours) and signals. Thus I have no jumpers, and no vias that exist just for the purpose of routing a network to the opposite side. (But not that it would matter! A signal, power or ground trace having to go to the other side and back has no effect at DC or audio frequencies. Stray inductances of of vias and such are another RF consideration.)

There is a small exception to the signals being on the bottom: late in the design I decided to add a stereo/mono switch, and some of the traces for that ended up in the top copper.

The finished unit is very quiet, and the sound quality is terrific.

If you have a good, dual-voltage power supply, quiet, distortion-free audio mostly boils down to the choice of op-amps more than anything else (I used NE5532's from ON Semiconductor), avoiding extremes like excessively low or unnecessarily high input impedances, and good supply bypassing.

\$\endgroup\$
3
  • 2
    \$\begingroup\$ I think this is a bit misleading. Audio circuits don't have RF frequency components in their signal, but that does not mean that RF interference can simply be ignored. Active circuits not designed for RF frequencies can do all kinds of bad things when exposed to them. They could get rectified and the result added to the signal. Active power supply rejection or common mode rejection circuitry breaks down at those frequencies, eventually introducing artifacts. Good grounding matters even at audio frequencies due to high S/N required. Return currents can cause offset voltages. \$\endgroup\$ Commented Nov 29, 2012 at 14:42
  • 2
    \$\begingroup\$ A quickie test for RF rejection of audio circuits is to wave an active GSM phone around the circuit. If it is rectifying radio signals, you will hear that familiar intermittent buzz in the audio. \$\endgroup\$
    – markrages
    Commented Nov 29, 2012 at 22:04
  • \$\begingroup\$ I was going to write about star grounding in the answer, but I didn't bother. It might not be necessary in small signal processing stuff where you don't have big return currents. \$\endgroup\$
    – Kaz
    Commented Nov 30, 2012 at 4:20
4
\$\begingroup\$

There is no need to agonize of power routing if the power supply is locally bypassed to the ground plane at each place it is used. The problem that circuitous power traces causes is to make the apparent power supply impedance higher. A local bypass cap is a low impedance shunt, thereby locally bringing the impedance back down.

In fact for circuits that require high signal to noise ratio like audio, you might want to add a little deliberate impedance in the form of a ferrite bead or "chip inductor". These would be in series with the power supply feed but before the bypass cap to ground. The inductor and cap form a low pass filter. This keeps high frequencies off the power pin of the local device. This is good because beyond some frequency, the device's active circuits no longer work to get you good power supply rejection ratio. The active circuits handle the low frequencies in the power supply feed, and the inductor/capacitor filter attenuate the high ones.

In cases like this, the cap is really more of a filter than a bypass. In other words, the 300 MHz performance isn't so critical, but you want the capacitance to be high enough to make a reasonably low rolloff frequency with the inductor. For example, I'd use a 10 µF ceramic where for a digital circuit I might use a 1 µF or 100 nF in really high speed cases.

\$\endgroup\$
3
\$\begingroup\$

Like everything in engineering the correct answer is that "it depends." That said, here are some general guidelines based on the underlying physics.

Ceteris Parabis, your approach #1 is universally superior. The stronger (larger, more contiguous, hopefully better stitched) reference plane will minimize the circulating current's magnetic loop area. The increased length (and separation) of the "power" rails is insignificant since all that matters in the area of the loop formed in 3D between the traces carrying the outbound and returning current. If those traces are always over the reference plane (a product of the plane being largely continuous and covering the bottom surface of the board), then the loops are minimum by definition -- that's just geometry. If you want to be really pedantic, then you could balance (make the total length the same) the positive and negative power rail tracks.

Obviously, I'm assuming here that the overall size of the board is small, the width of your tracks is sufficient for the power you are trying to deliver, and the materials appropriate for the voltages you encounter (at +/-12 the common stuff works just fine).

When confronted with your two scenarios, the general strategy should always be to optimize the reference ("ground") plane, since there is literally nothing you can do to further filter it once noise compromises the surface. Whereas, bypass capacitors, other forms of passive or active filters, and layout separation techniques can all be effectively applied against noisy power pathways (when you can compare them to a quiet reference plane).

@Kaz's advice about the low-frequencies of audio implying no need for RF attention is actually a bit misleading. While it is true that many audio circuits are apparently unaffected by RF interference, that is the result of a number of conscious design choices, not something inherent to working with audio signals. In fact @Kaz goes so far as to recommend "good supply bypassing," which is itself a counter-RFI technique (you are implementing a Low Pass Filter (LPF) by forming a first order filter from the trace impedance and the installed capacitor). Power supply decoupling in it's most common form is largely ineffective against audio-band signals (you rely on the bulk output capacitance of the power source for that). The decoupling handles the high-frequency (RF) harmonics generated from transient events, hence the name (to decouple the high and low frequency components of the power signal).

Further, you must use audio bandwidth limited operational amplifiers (virtually none of what you think of as "audio" amplifiers are bandwidth limited to just audio frequencies due to the need to support gain) or you face a situation of vulnerability with a high gain, high impedance amplifier. If your amplifier has an input impedance of 10-MegaOhm and a gain of 100X, what happens when your PCB trace picks up 1 *NANO*Amp of current from a nearby RF source? Yeah, you just coupled 1-VOLT of noise into your output.

In general, it is never a good idea to not follow good layout practices. Any board that works, will work better with RFI mitigation applied.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.