PGA2311 / OPA1632 Balanced Level Controller

Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
Hi All,


I'm looking for feedback on a first rev PCB design for a PGA2311 volume controller run differentially (i.e: balanced) with OPA1632 as input and output buffers. I don't have a real schematic drawn up as I'm working from the data sheet recommendations. Hopefully I'm providing enough info. I've prototyped the digital side with a though-hole PGA chip and single ended signals.

Here's an album of the PCB layers:
https://goo.gl/photos/3FPrTtyCsy9ceFTo9


  • The board will take in a regulated 5vDC supply that will be converted to +/-5vDC using a CUI DC-DC converter that is filtered with caps and radial inductors at the input and outputs. The incoming 5vDC also provide digital power to the PGA chip and can back feed to the uController which is off-board.
  • There are 2 circuit grounds but only one ground plane. I split the ground in the lower right corner, the larger portion is for audio ground and the smaller for digital.
  • The OPA1632 can take a single ended or differential signal and drive the two inputs of the PGA chip with a differential signal, lowering even-order distortion
  • The OPA1632 PCB layouts are based on high-frequency recommendations from the LMP8350 data sheet, including the removal of ground and power planes from beneath the chip and feedback resistors
  • The resistors are 0805 package and there are similarly sized caps for PS decoupling close to the pins
  • The output connectors are just left of center with 1206 package resistors in series, I'll populate with something around 100 ohm.
  • The 2x4 header in the lower right connect to a microcontroller
  • The "-" symbols indicate a via to the ground plane. The ground plane is split to isolate the incoming supply voltage and digital.
  • The "+" go to the power plane. The power plane is split like the ground plane but part of it is unused, I guess I should ground the unused portion.

Datasheets
http://www.ti.com/lit/ds/symlink/pga2311.pdf
http://www.ti.com/lit/ds/symlink/opa1632.pdf
http://www.cui.com/product/resource/pqmc3-s.pdf


I'm surely leaving something out but I've been looking at this for too long and need some outside opinions.

Brian
 
Last edited:
I'm a bit confused, but I didn't look very closely either. You say you have a power and ground plane, but you have +5V and -5V supplies. That's three 'planes', +5V, -5V and ground.

Also, you route the ground sides of bypass caps to a central ground spine with simple top side traces. Why not a short stub to a via directly to the ground plane? Those thin and long top side traces are extremely inductive, and not needed if you have some wide foil that you can drop a via to, not even an entire layer as a plane.

I've found that using two inner layers for power and signals, along with a top and bottom signal layer with a ground pour can work well. You won't have 'planes' but by finessing the layout, you can get a lot of continuous foil where you need it, enough for 2 power foils and ground, along with vertical and horizontal signal routing. This, with enough vias, can route things well.
 
I'm a bit confused, but I didn't look very closely either. You say you have a power and ground plane, but you have +5V and -5V supplies. That's three 'planes', +5V, -5V and ground.

OK, I probably explained my approach poorly. I have 3 power rails and 2 grounds in the circuit: Digital +5 which also feeds the inside of the DC-DC converters; isolated +/-5vDC for the audio rails. I am maintaining 2 grounds, 1 for digital/incoming power and 1 for audio. This is why the ground plane is split in the lower right corner. I am not using the power plane to distribute the audio rails at all... if I could get a board with 3 internal planes I would have done that but because I only a single power plane I chose to route the audio supply rails on the top and bottom layer. The power plane has some areas where it is facilitating the digital 5v but it is a bit underutilized.

Also, you route the ground sides of bypass caps to a central ground spine with simple top side traces. Why not a short stub to a via directly to the ground plane? Those thin and long top side traces are extremely inductive, and not needed if you have some wide foil that you can drop a via to, not even an entire layer as a plane.

I'm not following that. The 2 long traces running up the middle of the top layer are the +/-5V supply rails. The big radial electrolyitic caps are terminated directly to the ground plane. The SMD caps are close to the active devices and have short traces to individual vias to the ground plane. That doesn't mean I have it right, I just want to make sure we're talking about the same traces.

I've found that using two inner layers for power and signals, along with a top and bottom signal layer with a ground pour can work well. You won't have 'planes' but by finessing the layout, you can get a lot of continuous foil where you need it, enough for 2 power foils and ground, along with vertical and horizontal signal routing. This, with enough vias, can route things well.

Unfortunately my software and supplier do not permit traces on inner layers.
 
If I were you I would move analog power entry to the left side of the board. This will give you freedom to properly route digital side signal and power. I do not know how restrictive is your software but you need dedicated digital ground plane or at least a copper pour of decent size to go under the PGA chips and all the digital signalling. As it has already been suggested to you earlier by Monte McGuire you should reconsider those tiny power and ground traces feeding the digital side of the PGA chip as well.

Also when you route power to the analog and digital side of the PGA chip your power traces should first hit the bypass capacitor and from the bypass capacitor go to the corresponding IC power pin. Connecting the incoming power trace between the bypass capacitor and the IC's power pin is discouraged in all PCB routing guides. Also keep in mind the fact that GND connection should have much lowest inductance than the power feed which you totally ignored on the digital side power routing.

Hope it helps.

Regards,
Oleg
 
Last edited:
Much better. One question, why do you change layers for analog power rails... twice? Just keep them in "green" layer and save a lot of vias.

You can also turn the digital side connector by 90 degrees and save even more vias there. Using vias is not criminal but I would recommend to minimise their use where possible.

You can place decoupling capacitors much closer to the PGA2311 power pins if you move them to the underside of the PCB. The board is only 1.6mm thick and this is how close those decoupling capacitors can be to their respective pins.

Looking at how much unused PCB area you have there suggests that you can make your PCB significantly smaller.
 
Much better. One question, why do you change layers for analog power rails... twice? Just keep them in "green" layer and save a lot of vias.

You can also turn the digital side connector by 90 degrees and save even more vias there. Using vias is not criminal but I would recommend to minimise their use where possible.

You can place decoupling capacitors much closer to the PGA2311 power pins if you move them to the underside of the PCB. The board is only 1.6mm thick and this is how close those decoupling capacitors can be to their respective pins.

Looking at how much unused PCB area you have there suggests that you can make your PCB significantly smaller.

That's right. I had jumped planes because the power rails intesected the digital path. Not a problem anymore so I'll consolidate. The board size is actually fixed to 2.5x3.8" because I buy through a prototyping program.

Sent from my SM-N900V using Tapatalk
 
That's right. I had jumped planes because the power rails intersected the digital path. Not a problem anymore so I'll consolidate. The board size is actually fixed to 2.5x3.8" because I buy through a prototyping program.

Sent from my SM-N900V using Tapatalk

Actually, because the opamps are oriented differently the lines have to criss-cross too much to stay in the same plane. I'm going to move one of the rails to the power plane.
 
I made some more adjustments. I realized I could use the power plane for both rails easily because of the way they were previously routed straight down the middle. The power plane is now in four sections. The digital power will come straight from a microcontroller GPIO pin due to the low current required.

https://goo.gl/photos/KuvzJ3FrrqMV8eWo6

I'm thinking I'll order boards this weekend so I'd really appreciate some error checking.
 
Power and ground planes are great for high frequency and high speed digital systems but they are unnecessary for base band audio gear. Nothing wrong with using them and it does greatly simplify PC board layout.

But multi-layer boards are considerably more expensive to make. Nothing wrong with basic dual sided for audio.

FWEIW, I make my own PC boards for simple projects and use single sided as I have no facility to plate through holes. I use zero ohm resistors for jumpers. Again at audio frequencies, that is just fine.

P.S. My flame suit here is that I do design digital video devices in my day job. latest stuff is 12gbs for 4K video. So, yes I am fully aware of RF layout techniques. And that why I say it's a waste for analog audio projects.
 
For the record, since I hate when threads trail off into nothing, I wanted to report back that I pulled this through to the finish line. The forum won't seem to let me embed images so here's some links.

Solder paste and components:

https://goo.gl/photos/RVxTCyqsQsmPao4N7

After flowing, through-holes parts and wiring:

https://goo.gl/photos/3FqAZkBcA1SVKz4m9

Sounds nice, thanks for all the help

Brian
 
Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.