My first DAC attempt...PCB help needed

[ezkcdude]

Hey, all. I've been working the last several days on designing a PCB for my DAC. For a look at the schematic (the PCB strays somewhat), see:
http://www2.kumc.edu/students/ezamir.../schematic.png

As for the PCB, it is basically the fairly common (it seems to me) topology of CS8416->AD1896->PCM1794(8) and then AD8610 for I/V conversion. It uses 3 LM317's (3.3, 5.0, 12) and 1 LM337 (-12), and will be input a +/- 15V line from a dual supply DIY PSU I made recently. See my web page for more info. Thanks, in advance, for any advice/suggestions yada, yada.

[Chris Jennings]

Hi.

The filter components for the PLL on the CS8416 should be mounted much closer to pin 8. Refer to the data sheet (page 59) for details.

http://www.cirrus.com/en/pubs/proDat.../CS8416_F1.pdf

The pll filter is important on achiving good jitter rejection.

HTH

Chris

[ezkcdude]

Thanks, Chris.

[ezkcdude]

I've updated the PCB. I guess it must be perfect, since there were no other comments besides Chris. Here's a link to the PCB showing all layers:
http://www.cellandtissue.com/DIY/DAC...cb_all_v01.png

For more pics showing the layers separately, please see my www (middle of the page).

I hope it is clear my comment about the PCB being perfect is pure (wishful?) sarcasm.

[Ulas]

The combination of fine-pitch SMD and no solder mask makes ExpressPCB Miniboards very difficult to work with. I suggest you increase the pad clearance (in board properties) to at least .020" and define all pads that connect to a filled plane as thermal pads.

I prefer the ground plane on the component side, wide power busses, and 0603 SMD passives on either side to reduce trace length.

[ezkcdude]

Originally posted by Ulas
The combination of fine-pitch SMD and no solder mask makes ExpressPCB Miniboards very difficult to work with. I suggest you increase the pad clearance (in board properties) to at least .020" and define all pads that connect to a filled plane as thermal pads.

I prefer the ground plane on the component side, wide power busses, and 0603 SMD passives on either side to reduce trace length.

Thanks. Do most people agree that ground plane should be on the component side? If so, does that mean the bottom should be used for power rails/planes? That's a major change, so it would be great if other people could chime in their opinion on this.

[Ulas]

EZ, don’t change your layout on my account. I was just stating MY preferences. Understand, unless you are experienced soldering SMD, the ground plane on the component side will make assembly much more difficult. It will also necessitate more vias, which may bump against the 250-hole per board limit.

[ezkcdude]

Thanks. I have a quick question. What is the benefit of specifying the thermal pad connections?

[dsavitsk]

Originally posted by ezkcdude
Do most people agree that ground plane should be on the component side? If so, does that mean the bottom should be used for power rails/planes?

Yes and Yes. If you search around there is a good article by Guido Tent on the subject.

Also, as you have things now, I would work very hard to get those big cuts out of the groundplane. It may take moving some stuff around, but they are a bad thing.

Also, I like to include ferrites/inductors (0805 or 1206) on the power rails close to the power pins. Not only does this clean up the power, but it will give you some little places to cleverly route some traces.

And why do G1/G2/RG/LG, etc. not just connect to the ground plane? Why the little extra? Oh, and add a couple of vias to the ground and power rails to allow easier metering.

I would also space the spdif and V and output connections about 5mm (or 5.08mm) apart so that you can use a terminal block. You'll thank me later.

Last, I know you probably think space is too tight, but I would add an input transformer and perhaps a little buffer. It will do more to improve the sound that just about anything else. There is a schematic floating around that uses the 74HC04D that is attributed to a now banned member. The same schematic can also be found in the Philips datasheet for that part.

And, for what it's worth, I find the boards without soldermask a little easier to solder SMD onto. Not sure why, exactly, but things always seem to come out cleaner for me.

-d

[ezkcdude]

D, thanks for your advice. Let me take these points one by one.

Also, as you have things now, I would work very hard to get those big cuts out of the groundplane. It may take moving some stuff around, but they are a bad thing.

If you have any ideas how to re-route some of those signal traces between AD1896 and PCM1794, I'd love to hear about it. I couldn't see a way to avoid using the vias there.

Also, I like to include ferrites/inductors (0805 or 1206) on the power rails close to the power pins. Not only does this clean up the power, but it will give you some little places to cleverly route some traces.

I should have some ferrites. I'm just not sure how to do that. Do they go between the rail and ground just like decoupling caps?

And why do G1/G2/RG/LG, etc. not just connect to the ground plane? Why the little extra?

Not really by choice. I think it is a problem with ExpressPCB and choosing the wire connector. Maybe I should just make them large vias instead.

I would also space the spdif and V and output connections about 5mm (or 5.08mm) apart so that you can use a terminal block. You'll thank me later.

Yeah, I plan to do this, although I just tried terminal blocks on my other PSU project, and I didn't like them. Do you know of any high quality blocks that are spaced at 5 mm.

Last, I know you probably think space is too tight, but I would add an input transformer and perhaps a little buffer. It will do more to improve the sound that just about anything else. There is a schematic floating around that uses the 74HC04D that is attributed to a now banned member. The same schematic can also be found in the Philips datasheet for that part.

I'm sure these are great suggestions for more experienced DIYers, but since this is my first project, I'd rather stick to what I (sort of) understand. Transformers and buffers are a little too complex for me to get a handle on at this point. (And, yes, I think the space is already really tight. Good I have small hands, though!)