Author Topic: Need pcb layout review please  (Read 328 times)

0 Members and 1 Guest are viewing this topic.

Online hummusdude

  • Regular Contributor
  • *
  • Posts: 79
  • Country: us
Need pcb layout review please
« on: April 17, 2021, 03:57:50 am »
This is my first board so I'm sure it has some issues. It's an audio pre-amp with active 2-band tone. I made this to go with a power amp design I found online. I intend to put it in the case with the power amp. The power supply for the power amp is beefy and puts out +- 25VDC so I'm using that to supply this pre-amp board. For fun I added some different controls to trigger the microcontroller. The Nano is used just to control the dpot that controls the gain of the pre-amp, and to drive the shift registers that control the two 7-segment displays.

Some questions I have...

Is the 5VDC linear regulator too close to the analog section?

I tried to keep all of the signal lines on top but there a couple of exceptions. Is that okay?

Does it make a difference in the overall power dissipation if I supply the 5V linear regulator from 15VDC or 25VDC? I understand the power loss issue but not sure if it matters in this case.

The treble/bass controls are potentiometers that I will panel mount on the front of the case. Is it okay to twist all three wires for the run from the front panel to the board connections?

 

Offline FriedMule

  • Frequent Contributor
  • **
  • Posts: 697
  • Country: dk
  • Can make even the simplest task look imposible.
Re: Need pcb layout review please
« Reply #1 on: April 17, 2021, 05:47:29 pm »
Please understand that I am propperly more noob than you but I have been guided trough some amplifier designs. :-)

As I see your layout would I suggest that you maybe should try to shorten your traces as much as possible and widen your power traces as much you can.
Maybe you should think of using a 4 layer board (signal, ground, power, signal)?
Your usage of via is fine but I think you can avoid that with a different layout.
Even if I appear online is it not necessary so, my computer is on 24/7 even if I am not on.
 
The following users thanked this post: hummusdude

Online dietert1

  • Frequent Contributor
  • **
  • Posts: 893
  • Country: de
    • CADT Homepage
Re: Need pcb layout review please
« Reply #2 on: April 17, 2021, 08:49:58 pm »
Did you make and test a prototype? The digital pot you selected isn't the best choice. Everybody wants a logarithmic pot in this application and a display in dB.
Also, if this is meant to be a compatible audio preamplifier with RCA inputs, input impedance should be about 47K or above. In your circuit it may be as low as 4K7 depending on the balance setting. By the way, if you use a logarithmic digital pot like PGA2310, balance control can be implemented in software. The input circuitry should have some EMI filters, at least the usual 1K with 1nF low pass.

Regards, Dieter
 
The following users thanked this post: hummusdude

Offline strawberry

  • Frequent Contributor
  • **
  • Posts: 346
  • Country: lv
Re: Need pcb layout review please
« Reply #3 on: April 17, 2021, 09:32:09 pm »
PCB
too many unnecessary vias
unnecessary thin traces and TH pads
trace between dip pins (too little space in this example)
SCH
7seg display resistor array or network
 
The following users thanked this post: hummusdude

Offline mariush

  • Super Contributor
  • ***
  • Posts: 4070
  • Country: ro
  • .
Re: Need pcb layout review please
« Reply #4 on: April 17, 2021, 10:17:55 pm »
Voltage regulators.

Add 0.1 uF or 0.01 uF ceramic capacitors on the input of both +15v and -15v regulators.
Add a small electrolytic input capacitor on both +15v and -15v regulators ... small as in let's say 10..100uF, anything higher won't help more
No idea why you went with 2.2uF , it's a weird value and unnecessarily small.
Below some uF value all capacitors will have the same diameter and height, so you're not saving pcb space and you don't have to be exactly as the datasheet minimums recommend.
I'd suggest going with a value that you're gonna reuse in the circuit somewhere else... for example 22uF 35v rated electrolytic capacitors which you can use for the opamps as well.

I'd add output capacitors to both +15v and -15v regulators... again, don't understand why go with 100nF on one and 1uF on the other... I'd go with 10uF 25v electrolytic on both, or reuse 22uF 35v you already picked for the input and output and opamps.

I wouldn't use electrolytic capacitors with less than 10uF capacitance, and if I have to I'd use ones with high voltage rating, like 35v..50v, to get better specifications.

If the 5v regulator's gonna be physically very close to the 15v regulator output, then you don't need input capacitors for it, as the output capacitor of that regulator will provide the capacitance and the voltage should be smooth enough to not require decoupling capacitors.

The opamps ... the 22k resistors bother me a bit ... do you have to use 22k or could you maybe deal with 10k (in which case you could use 2 10k in series and simplify your bom by having only 10k resistors)

the actual layout ... i'd use thick traces for +25v and -25v and i'd route them horizontally to the left of the connector, and  rotate by 90 degrees both regulators so if you wanted to you could place heatsinks on the edge of the board. Probably your board doesn't consume that much current, but never hurts to have the option.

The 5v regulator could fit between the +15v one and the input power connector which could be moved a bit to the right.
Then you'd have room to move up that mcp4231 and not have such long traces from the arduino to it.

I'D move the bass and treble headers to the left edge, like the out terminal, and maybe rotate 90 degree the opamps to have the traces go directly to it.

I see you have footprints for ceramic capacitors for 22uF ... I hope you're aware capacitance of ceramic caps varies with voltage and also that 22uF capacitors with high enough voltage rating will be expensive.
If you need the 22uF may be better to use electrolytic capacitors or maybe consider having 2-3 footprints for 10uF ceramics in parallel.


Rotate ir header and rotary header so they're on the edge
do something with the shift registers and the 7segment header ... move a bit to the right, rotate the shift registers, use resistor arrays if you have to or smaller footprint resistors




 
The following users thanked this post: hummusdude

Online hummusdude

  • Regular Contributor
  • *
  • Posts: 79
  • Country: us
Re: Need pcb layout review please
« Reply #5 on: April 18, 2021, 01:02:23 am »
Did you make and test a prototype? The digital pot you selected isn't the best choice. Everybody wants a logarithmic pot in this application and a display in dB.
Also, if this is meant to be a compatible audio preamplifier with RCA inputs, input impedance should be about 47K or above. In your circuit it may be as low as 4K7 depending on the balance setting. By the way, if you use a logarithmic digital pot like PGA2310, balance control can be implemented in software. The input circuitry should have some EMI filters, at least the usual 1K with 1nF low pass.

Regards, Dieter

I breadboarded it and tested it separately and while hooked to the power amp components as well. As for inputs, this is intended to be a low-gain pre-amp to boost the output of my phone/laptop. The designer of the power amp has a device that goes to 1V pk output but mine only goes to 660 mV. I know I could change the gain of the power amp but I wanted to do this for practice and fun.

I also wondered about the lack of coupling caps at the front end. The source of the circuit claims it is very quiet and when I breadboarded this it was. I tried a few different values of cap on the input but everything adversely impacted the response of the tone circuit so it seemed prudent to go with the original design since it was working as described with very low noise.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf