PCB Design Feedback

[King Penguin]

Hello,

I am building a Nixie tube clock and want to integrate speakers. I am using the PCM2912A as a USB Audio Codec, the TDA7375V for the audio amplifier, and the ATMEGA328P for controlling the Nixie tubes. Due to both the ATMEGA and PCM ICs requiring a USB connection I am using the USBLC6 for ESD protection, the ADUM3160BRWZ for power isolation between the USB bus and 12V (which will be used for powering the Nixie tubes), and the FE1.1S as a USB hub. I am posting the schematic for the USB controllers (not the TDA and ATMEGA ICs) and their respective layouts. I am new to PCB layout and I tried the usual techniques like putting the decoupling caps close to the ICs, short connections, etc, but I am not 100% sure since I am dealing with USB 2.0 and not just low-frequency signals. Any advice and/or suggestions are welcomed.

Chris

[ahsrabrifat]

USB 2.0 high-speed signals (D+ and D−) should have a 90Ω differential impedance. Signal reflections could degrade performance if your PCB stack-up doesn’t ensure this.  D+ and D− traces must be equal in length to prevent skew. Even a small difference can cause signal integrity issues. Avoid sharp 90° turns (use 45° bends or smooth curves). Keep the differential pair close together and avoid vias if possible.
Keep them away from noisy signals, especially the 12V power traces. Since you're dealing with an audio circuit (PCM2912A), it's essential to prevent noise coupling by keeping separate ground planes for USB, digital, and analog sections. Route USB ground return paths carefully to prevent ground loops. The PCM2912A analog GND (AGND) should connect to the digital ground (GND) at a single point near the codec. If possible, run a simulation or check impedance with a PCB manufacturer before fabrication can help prevent issues. Since you are making a nixie tube clock, here is a clock PCB design that you can see for further reference.

https://www.pcbway.com/project/shareproject/Nixie_Clock_8690fad1.html

This clock has been working for 6 years without any problems.

[tooki]

I’m not sure the digital isolator is really necessary. It certainly isn’t needed just to have different supply voltages. (I don’t see where 12V appears anywhere.)

I assume you’re using ground pours that aren’t shown here?

Two minor “formal” things that are easy to fix:
1. Use component designators correctly and consistently. Having resistors, capacitors, and connectors that use the “U” designator prefix is extremely bad form.

2. In the schematic you have things overlapping to the point the text cannot be read. Move things around to avoid this. I know EasyEDA’s default resistor symbols and text sizes, for example, are big enough to easily get in the way on adjacent pins, so you need to stagger adjacent pins. A schematic where one cannot read component designators and values, or net names, isn’t very useful.

[mtwieg]

Hard to say if the isolator is appropriate without knowing more about the high power side of the circuitry. But if you're going to put in an isolation barrier, I would probably want as much of the logic on the "safe" side of the isolation barrier as possible (i.e. everything on that schematic would be on GNDU and not GND).

Do you need to support USB high speed or just full speed? For just full speed, impedance and skew on the USB lines isn't an issue. For high speed, you will need to be very careful and will likely need a four layer stackup.

[King Penguin]

I’m not sure the digital isolator is really necessary. It certainly isn’t needed just to have different supply voltages. (I don’t see where 12V appears anywhere.)

The 12V power supply is needed to power the dedicated TDA7375 audio amplifier since I don't trust the motherboard USB will be able to supply the necessary current. I did not include it in the schematic for simplicity reasons. PCM2912 is not capable of driving the speakers I want to use. So the stereo output of the PCM IC will be the input of the TDA7375 amplifier through some decoupling capacitors. I'll try to fix the schematic issues as you mentioned, thanks.

Hard to say if the isolator is appropriate without knowing more about the high power side of the circuitry. But if you're going to put in an isolation barrier, I would probably want as much of the logic on the "safe" side of the isolation barrier as possible (i.e. everything on that schematic would be on GNDU and not GND).

Do you need to support USB high speed or just full speed? For just full speed, impedance and skew on the USB lines isn't an issue. For high speed, you will need to be very careful and will likely need a four layer stackup.

USB 2.0 high-speed signals (D+ and D−) should have a 90Ω differential impedance. Signal reflections could degrade performance if your PCB stack-up doesn’t ensure this.  D+ and D− traces must be equal in length to prevent skew. Even a small difference can cause signal integrity issues. Avoid sharp 90° turns (use 45° bends or smooth curves). Keep the differential pair close together and avoid vias if possible.
Keep them away from noisy signals, especially the 12V power traces. Since you're dealing with an audio circuit (PCM2912A), it's essential to prevent noise coupling by keeping separate ground planes for USB, digital, and analog sections. Route USB ground return paths carefully to prevent ground loops. The PCM2912A analog GND (AGND) should connect to the digital ground (GND) at a single point near the codec. If possible, run a simulation or check impedance with a PCB manufacturer before fabrication can help prevent issues. Since you are making a nixie tube clock, here is a clock PCB design that you can see for further reference.

https://www.pcbway.com/project/shareproject/Nixie_Clock_8690fad1.html

This clock has been working for 6 years without any problems.

The PCM2912 datasheet says full-speed but I'll look more into USB layout techniques just to be on the safe side. Thanks for the input and resources.

[tooki]

I’m not sure the digital isolator is really necessary. It certainly isn’t needed just to have different supply voltages. (I don’t see where 12V appears anywhere.)

The 12V power supply is needed to power the dedicated TDA7375 audio amplifier since I don't trust the motherboard USB will be able to supply the necessary current. I did not include it in the schematic for simplicity reasons. PCM2912 is not capable of driving the speakers I want to use. So the stereo output of the PCM IC will be the input of the TDA7375 amplifier through some decoupling capacitors. I'll try to fix the schematic issues as you mentioned, thanks.

Current or voltage?

USB can’t provide the 8-18V supply voltage required by that amp, so the current draw as such becomes irrelevant. However, since you describe the project as a clock with integrated speakers, I imagine that we aren’t talking about a home theater system here, so your chosen amp chip may be overkill. You might be surprised what a lowly PAM8000-series with 5V supply is capable of! (Even if we ignore the silly specs at 10% THD, you can still get over 2W into 4 ohm speakers, or over 1W into 8 ohms, with 1% THD.) If we are just talking about clock radio type of volume, something like that would be plenty.

Since you haven’t shared many of your design considerations/requirements, it’s hard to give concrete advice, but consider that with a modern class-D amplifier, your amp power requirements would drop significantly. (Most class-D amps still need more than 5V for higher power levels, though there are exceptions*.)

If we assume 12V, then a whole world of efficient class-D amp chips opens up. I have personal experience with the TI TPA3126D2 (and other members of that family of chips) and they’re great. I don’t see any reason to use an antiquated linear amplifier chip.


* If I were designing a USB (or Bluetooth) speaker today, I would use a USB (or Bluetooth) codec with I2S, SPDIF, or other digital output, going directly to a class-D amplifier with corresponding digital input. Avoiding an analog signal chain entirely significantly reduces the chances of interference in the output.


I asked you earlier:

I assume you’re using ground pours that aren’t shown here?

This wasn’t a rhetorical question. Grounding is a critical part of PCB layout, so we can’t fully examine your layout if it’s missing.

[King Penguin]

I’m not sure the digital isolator is really necessary. It certainly isn’t needed just to have different supply voltages. (I don’t see where 12V appears anywhere.)

The 12V power supply is needed to power the dedicated TDA7375 audio amplifier since I don't trust the motherboard USB will be able to supply the necessary current. I did not include it in the schematic for simplicity reasons. PCM2912 is not capable of driving the speakers I want to use. So the stereo output of the PCM IC will be the input of the TDA7375 amplifier through some decoupling capacitors. I'll try to fix the schematic issues as you mentioned, thanks.

Current or voltage?

USB can’t provide the 8-18V supply voltage required by that amp, so the current draw as such becomes irrelevant. However, since you describe the project as a clock with integrated speakers, I imagine that we aren’t talking about a home theater system here, so your chosen amp chip may be overkill. You might be surprised what a lowly PAM8000-series with 5V supply is capable of! (Even if we ignore the silly specs at 10% THD, you can still get over 2W into 4 ohm speakers, or over 1W into 8 ohms, with 1% THD.) If we are just talking about clock radio type of volume, something like that would be plenty.

Since you haven’t shared many of your design considerations/requirements, it’s hard to give concrete advice, but consider that with a modern class-D amplifier, your amp power requirements would drop significantly. (Most class-D amps still need more than 5V for higher power levels, though there are exceptions*.)

If we assume 12V, then a whole world of efficient class-D amp chips opens up. I have personal experience with the TI TPA3126D2 (and other members of that family of chips) and they’re great. I don’t see any reason to use an antiquated linear amplifier chip.


* If I were designing a USB (or Bluetooth) speaker today, I would use a USB (or Bluetooth) codec with I2S, SPDIF, or other digital output, going directly to a class-D amplifier with corresponding digital input. Avoiding an analog signal chain entirely significantly reduces the chances of interference in the output.


I asked you earlier:

I assume you’re using ground pours that aren’t shown here?

This wasn’t a rhetorical question. Grounding is a critical part of PCB layout, so we can’t fully examine your layout if it’s missing.

Yes, I do have ground pours and a grounding plane directly below the signal traces. I thought it would be best though to disable it from the view port in order for the traces to be clearly visible, especially on the lower layers.

The project is targeted for casual PC use, listening to YT, Spotify, etc, and not high-end, that's also the reason why I did not share any specifications for the audio amp and speakers, it seemed irrelevant information since it is not for professional use and there aren't any real specifications. Having not worked with a high-speed layout, I wanted to minimize the possible points of system failure. Dropping into lower and more manageable frequencies seemed like a good idea (hence the use of the analog signals and amplifier), even if it meant a small degradation of the audio quality since it is more generic use and not studio-level applications.

I will check the motherboard manual to see if it mentions what current can it safely output and reconsider going digital.

The reason I wanted to use a 12V power supply is because the Nixie tubes require 160V and 2mA to operate. I have 4 of them. the PCB already includes a DC-DC boost converter to step up 12V to 160V. All in all the USB port would need to power the Nixie tubes themselves, the DC-DC boost converter, the USB controllers, the Arduino, and the amplifier. I am aware of the switching noise. The USB controllers would be powered from an LDO to filter out some noise along with the decoupling caps on the pins of course. Additionally, the physical distance on the board between these ICs is relatively large >30cm along with ground pours on the top layer between them.

I admit I did not look into what sort of power a 5V class D amplifier would draw. I just didn't want to load the port too much and that's why I used a separate 12V power jack especially, after I learned that USB power isolators are a thing and I didn't have to worry as much about the two GND nodes from each power source being at different potential relative to each other.

I have attached a 2D image of the PCB. It is 400x170mm in dimensions, on the left is the DC-DC converter, and on the bottom right are the USB controllers. In the middle is the audio amp along with a number of filtering capacitors for the power supply pins. On the top are the nixie tubes along with some driving ICs. The entire PCB and the rest of the circuit are relatively large and I thought to keep the initial post clean and to the point, hence the limited information. Sorry for the headache.