2
\$\begingroup\$

I'm designing my first PCB (two layer), the project is for an amplifier based on OPA2134.

The design/amplifier requires to have +12V, GND and -12V. The power for the amplifier comes from a USB-C->DCDC converter.

I'm having trouble defining the plane(s).

Should there only be a ground plane in the amplifier zone and then round +12V and -12V with wider tracks? Or should there be +12V power plane and -12V power plane and route the ground connections with wider tracks?

enter image description here

\$\endgroup\$
1
  • \$\begingroup\$ if nothing else, run a 1cm wide trace down the middle of the PCB, to be your GROUND. And don't cut that down in width, at any point. 1cm by 10cm (0.4" by 4") has 10 squares of foil, and the standard foil is 1 ounce per square foot, or 0.000498 ohms per square (at room temperature). That strip has 0.005 ohms (5 milli ohms) resistance and should serve just fine for an audio amplifier. \$\endgroup\$ Commented Aug 3, 2019 at 14:00

6 Answers 6

1
\$\begingroup\$

Choose the shape of the board so it fits in the enclosure and don't forget mounting holes.

If you use a 2 layer board:

Since you're using an isolated DC-DC converter for the power supply, put it on its own USB_GND mini ground plane, which will be isolated from the ground plane that is on the rest of the board. Make sure the ground plane is solid with no traces running through it.

The DC-DC converter may generate some HF noise so it would be a good idea to put it as far away from the inputs as possible. Lower left corner would be better. You can also add a LC filter in the output to get rid of the HF noise. Since current is only 40mA, no need for a huge power inductor, just use a ferrite bead with some hundred ohms impedance. To avoid ringing in this LC filter you can add a 1-2 ohms in series with the ferrite bead.

Opamps have very high power supply rejection (PSRR) at low frequency, and crummy PSRR at high frequency. So, an opamp does not care much about a couple extra ohms in series with the power supply, but it's important to keep the supply free of HF noise from the switching regulator.

Apart from that, note that 100nF thru-hole caps provide close to zero benefit. You use low value capacitors for good high frequency filtering/decoupling on your power supply. But that requires low inductance... and a thru-hole cap with 5.08mm pin spacing will have roughly the same inductance (about 4-6 nH) no matter what it is made of. In fact the standoff height between the base of the cap matters a lot more than the type of cap, since what determines inductance is loop area, in other words physical dimensions.

A tiny SMD ceramic cap has much lower inductance, thus much better performance, and this is ONLY due to the fact that it is tiny, low profile, and close to the board.

Also opamps do care about inductive impedance in the power supply, which can make them unstable. This is less of a problem for your opamp as it has only 8 MHz gain bandwidth, so this will be an easy layout opamp.

So basically:

Place the opamp

Put a ground plane, all traces on the other side.

Put 2 SMD 1µF 0805 or 1206 ceramic decoupling caps on one side of the opamp, with their ground connected to the ground plane at the same place, and route power to the opamp pins.

Put 2 electrolytics next to them, or further away, that's not really important.

No need for power planes, just use 1mm traces, it's only 40mA maximum.

Components in the feedback path should be close to the opamp.

Everything where HF performance matters should be SMD ; in this case that's pretty much just the input EMI filter caps and the filter caps on the output of the DC-DC converter.

Personally I'd use a filter like this on the output of the DC-DC, with 1µF MLCC caps.

schematic

simulate this circuit – Schematic created using CircuitLab

\$\endgroup\$
2
  • \$\begingroup\$ Why two parallele capacitors i your filter ? To lower their ESR ? \$\endgroup\$ Commented Apr 23, 2023 at 12:05
  • \$\begingroup\$ ESR, ESL, higher ripple current rating, and also quantity discount! 1µF is pretty cheap, got a tape of 100, it's faster and cheaper to put two than order 2.2µF \$\endgroup\$
    – bobflux
    Commented Apr 23, 2023 at 15:15
1
\$\begingroup\$

I'm also a newbee for designing PCB, but the trace wide depends functionally on the amount of current going through the traces. So in principle you should calculate it for both the 12V, -12V and GND traces what the minimum track width needs to be. Since your amplifier is powered from USB (which is like 0.5A maximum I believe), I don't think you will need thick trace widths.

Some people use wider track widths for GND, VCC and other power traces, just for 'clearity', to see at a glance which are data traces and which are not.

About planes, for what I know most people advise to use a ground plane. But if you can have a more clearer layout if you have a 12V and -12V power plane, I don't see any problem.

But there are experienced people here, maybe they have a better answer.

\$\endgroup\$
0
\$\begingroup\$

As the output current is limited to 40mA for a total supply current of about 44mA (when Iq is added) at 25C (which ultimately comes from the supplies) you could probably use reasonably wide tracks for power, provided they are decoupled as close as possible to the power pins.

OPA2134 short circuit current

A 10mm width track at 50mm length would incur a voltage drop of about 50 uV (I used the Saturn PCB toolkit) with negligible temperature rise.

I would personally use a ground plane under the device for noise reasons and to ensure the supplies can be decoupled as close to the device as possible.

\$\endgroup\$
0
\$\begingroup\$

Assuming a 4-layer board, I would have a ground plane and then split the power plane into +12 and -12 sections. Bypass the planes to ground near the chips.

This answer has some screen captures of how it is done in Altium.

But for an audio amplifier you can probably do it fine with just one or two layers.

\$\endgroup\$
0
\$\begingroup\$

With the USB power, keep the following in mind: image from the wikipedia
USB currentSo depending on your USB host port you will have limited current. Further as the other answers mention, make sure the GND plane is not cut down somewhere, and place +12V and -12V planes instead of tracks if you like more visual clarity.

\$\endgroup\$
0
\$\begingroup\$

A ground plane may be desirable for your blocking capacitors since it will sink and source and distribute power supply spikes better than the power rails. For your ground reference, you want to closely follow the signal path to avoid external magnetic fields coupling differently into signal and reference. If you have to add several signals coming via different paths from the same reference (like when adding the output of several preamps using the same panel ground), your reference input should also be a properly weighted (low-impedance) sum of incoming and outgoing reference. It may feel nonsensical to join several traces via 10ohms that are all connected at their other end anyway just to make for a reference ground. But hum doesn't care about "nonsensical".

Only by keeping bypass ground plane and reference ground tracks separate can you manage minimum susceptibility to humming along with minimum distortion due to crossover spikes.

A ground plane does not provide any worthwhile shielding from hum but it will help against mobile phone noise bursts.

\$\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.