pcm1792 I/V stage layout

[BrianGT]

I started my layout for my pcm1792 dac for my cdpro2 project. Here is my initial layout:
schematic
top layer
bottom layer
(it is a 2 layer board)

The I/V schematic is from the pcm1792 datasheet. Note: I haven't routed power to the differential summing opamp yet.

I have a few questions about this design:
1. Where can I find decent +15v and -15v regulators for the OPA627 opamps.
2. Should I regulate them seperately from each other, such as using seperate regulators for the left, right and differential summer, or would one regulator setup for all opamps work fine?
3. Is the power scheme that I choose to adopt, putting the capacitors on the bottom of the board alright practice?

Any comments/suggestions/criticisms are appreciated.

If anyone else is interested in this design, I can get some extra pcbs made when I am finished with this. I am doing this for my senior design project.

--
Brian

[Coulomb]

As I mentioned in my email Brian, I am interested in your project and would like some boards. If you need anything be sure to let me know.

Regards

Anthony

[jwb]

It's not going to matter much that the caps are on the bottom for power to a through-hole device. However I would strongly suggest that the power supply and filtering caps for the DAC must be on the top layer. Putting them on the other side will significantly degrade performance.

Not familiar with your CAD package, but why are you using the hash fill? Go for a solid pour instead.

This would work a lot better on a four-layer board. In your design you have pretty significant power supply loops. You are operating in the tens of megahertz: time to move up to four layers.

For regulators, a Sulzer with LM329 reference would be really nice. LT1085 adjustable would be cheaper and easier. LT1962 adjustable is a winner, too.

[BrianGT]

Originally posted by jwb
It's not going to matter much that the caps are on the bottom for power to a through-hole device. However I would strongly suggest that the power supply and filtering caps for the DAC must be on the top layer. Putting them on the other side will significantly degrade performance.

Not familiar with your CAD package, but why are you using the hash fill? Go for a solid pour instead.

This would work a lot better on a four-layer board. In your design you have pretty significant power supply loops. You are operating in the tens of megahertz: time to move up to four layers.

For regulators, a Sulzer with LM329 reference would be really nice. LT1085 adjustable would be cheaper and easier. LT1962 adjustable is a winner, too.

Thanks for your suggestions. I have made some changes, and updated the pictures. I managed to get all except for one trace of the dac power lines, on the top layer.

As for the hash fill, it was the default option with Protel, and looks pretty. I changed it to solid. It shouldn't make a difference for low frequency stuff.

As for the 4 layer board, I don't have the budget for this, unless you know a cheap place to get boards made.

Do you have any more suggestions for the layout? I am going to put some regulators on it soon. I will look into the ones you mentioned.

--
Brian

[jwb]

Ah, nice. I didn't understand before that both top and bottom planes are AGND. I'd say you have a few problems stemming from that. Notably, the top AGND and bottom AGND need to be connected by big fat vias in many places.

Take R40 for example. It is connected to AGND, and so is U1, but high-frequency signals are going to have a very hard time making the connection. The ideal return path is directly under the trace, back to pin 20. But on your board the signal has to squeeze between UL2 and UR1, all the way around UR3, back along the bottom of the board, snaking between pins 15 and 17, and finally back to pin 20. Whew! It's going to radiate like crazy.

If you put a fat via right next to R40 pin 2, the signal will be FAR happier. Also put a via under U1, at about pin 21.

For the same reason, I would horizontally flip C40, C41, and C42 (A and B), to make them closer to U2. Right now your +5V traces are like the Berlin Wall, dividing your ground plane into two parts. And the AGND pins of your capacitors are on the wrong side. They want to be on the same side of the wall as U2.

One other thing: I would change the IOUT traces to be the same width all the way to the opamp. Even though this is the analog side of the DAC, the signal still contains significant high-frequency components (otherwise, why would you need the LPF?). Any discontinuity can cause reflections and this distorts the signal.

Other than that it looks peachy I'm sure it's going to sound great. At this stage you are putting on the touches that separate your effort from the random taiwanese junk at circuit city. Close attention to detail here will result in superb sound in the final product.

[BrianGT]

Originally posted by jwb
Ah, nice. I didn't understand before that both top and bottom planes are AGND. I'd say you have a few problems stemming from that. Notably, the top AGND and bottom AGND need to be connected by big fat vias in many places.

Take R40 for example. It is connected to AGND, and so is U1, but high-frequency signals are going to have a very hard time making the connection. The ideal return path is directly under the trace, back to pin 20. But on your board the signal has to squeeze between UL2 and UR1, all the way around UR3, back along the bottom of the board, snaking between pins 15 and 17, and finally back to pin 20. Whew! It's going to radiate like crazy.

If you put a fat via right next to R40 pin 2, the signal will be FAR happier. Also put a via under U1, at about pin 21.

For the same reason, I would horizontally flip C40, C41, and C42 (A and B), to make them closer to U2. Right now your +5V traces are like the Berlin Wall, dividing your ground plane into two parts. And the AGND pins of your capacitors are on the wrong side. They want to be on the same side of the wall as U2.

One other thing: I would change the IOUT traces to be the same width all the way to the opamp.

Thanks for the suggestions. As for the ground planes, I need to remove them while working on the layout, and then I add them once I am finished. I plan on adding a lot of vias between the two ground planes, once I and through with the layout.

As for the Iout traces, they are 16mil coming out of the dac. Should I keep all the traces with them confined to 16 mil, instead of moving up to 30mil?

Also, any idea how wide I should keep the voltage traces? Should I keep them more uniform?

Thanks again for the suggestions!

--
Brian

[jwb]

Originally posted by BrianGT


Thanks for the suggestions. As for the ground planes, I need to remove them while working on the layout, and then I add them once I am finished. I plan on adding a lot of vias between the two ground planes, once I and through with the layout.

You might want to switch to Eagle, which is free and a little more reasonable than protel regarding poured polygons. Not on this project obviously

As for the Iout traces, they are 16mil coming out of the dac. Should I keep all the traces with them confined to 16 mil, instead of moving up to 30mil?

I would. Any change in trace width means a change in impedance and that means reflections. I guess you could work out the magnitude of the reflection to see if it's worth worrying about.

Also, any idea how wide I should keep the voltage traces? Should I keep them more uniform?

I usually just make them the same width as the pin at the origin. Or sometimes just round numbers like .025, .05, etc. I guess it doesn't really matter as long as the impedance is reasonable.

Cheers.

[BrianGT]

Originally posted by jwb

I would. Any change in trace width means a change in impedance and that means reflections. I guess you could work out the magnitude of the reflection to see if it's worth worrying about.

I usually just make them the same width as the pin at the origin. Or sometimes just round numbers like .025, .05, etc. I guess it doesn't really matter as long as the impedance is reasonable.

Cheers.

Thanks again, I made all traces the same size now, and added a bunch of vias. Any ideas on via placement? Is it the more the merrier, assuming that the shortest path to ground is the best.

Anymore suggestions?

--
Brian

[jwb]

Well in the real world every hole costs money. But no need for us prototypers to worry about that.

[MWP]

Thats pretty much identical to the IV stage i used on my DAC.
I also designed mine with Protel DXP.

http://www.overclockers.com.au/~mwp/dac3/

A few sugestions...

Get as many as of the DIP8 connecting tracks as possible on the bottom layer. Soldering top layer tracks can be a REAL pain if your using DIP sockets.

Use the default connection method of component pads to the ground pours... the "Relief Connect" style will make soldering them much easier and less messy.

This is a DIY project so although as tempting as it is to squash every up and make the PCB small, it is a better idea to space everything out a bit so later it is easier to change the design, etc without needing to make a new PCB.