Really not satisfied with layout need advice

[Yoshy]

Hello,

I'm really stuck with my layout and I'd like some advice on how to route and optimize the layout. This is supposed to be an integrated DAC with Chipamp Frontend.




Thanks
Phil

[pacificblue]

- Provide separate grounds (and terminals) for digital return paths, audio signal return paths and power supply return paths.
- You should provide fixing holes for the PCB.
- Turn C1 and C2 by 180°, so that the grounded pins are next to each other.

It is easier to give advice about a project with a schematic and known components.

[Yoshy]

Oh yes, I completely forgot ! Sorry I wasn't myself when I posted it seems

Schematics - PNG of DAC Chip

Schematics - PNG of Channels, Both are the same

[pacificblue]

Usually two layers are not enough for a DAC PCB. There are usually several power supply and ground layers on such a board. That provides the possibility to cross paths below surface mounted components.
It looks however, as if you were stuck still way before the layout, because the schematic is not even complete.
You will definitely have to add a lot of space to the left of the DAC, where you fit connectors and the 3,3 V power supply with decoupling capacitors right next to pins 8 and 9.
Add a power ground for the by-pass capacitors.
The by-passing is not complete. Refer not only to the voltage regulator datasheet, but also to the DAC datasheet. There need to be 100 nF right next to pins 15, 16 and 27, 28 plus 10 µF preferably Tantalum not too far away from there.
Do you really need two 5 V 1 A voltage regulators for <40 mA supply current? There are 100mA voltage regulators in surface mount and through-hole packages available.
Why do you need six ground connectors with 10 pins each? If this PCB will be the star-ground, the connectors should be placed next to each other and next to the power supply terminal to keep the ground paths short.
Turn C1 and C2 by 180° and make the ground connection from top to bottom layer between them, instead of at the power terminal.
It would look better, if you turned either ICA2 or ICB2 with all corresponding components by 180°. That is of course only for the symmetry, not for the function.

[Yoshy]

Originally posted by pacificblue
Usually two layers are not enough for a DAC PCB. There are usually several power supply and ground layers on such a board. That provides the possibility to cross paths below surface mounted components.

Yes, unfortunately, I don't know of any cheap 4-layers board houses

Originally posted by pacificblue
It looks however, as if you were stuck still way before the layout, because the schematic is not even complete. You will definitely have to add a lot of space to the left of the DAC, where you fit connectors and the 3,3 V power supply with decoupling capacitors right next to pins 8 and 9. Add a power ground for the by-pass capacitors. The by-passing is not complete. Refer not only to the voltage regulator datasheet, but also to the DAC datasheet. There need to be 100 nF right next to pins 15, 16 and 27, 28 plus 10 µF preferably Tantalum not too far away from there.

True but since I'm alone on this project I usually draw it up in schematics then, immediately, route it on the PCB - I'm not sure if this is really the way to go but this technique has proven it's ways for now at least for me that way I don't get a few thousand parts not routed at the end. This is why you see a lot of incomplete stuff. Here I got stuck with the chip amp part more; I don't like vias that much and I find some traces extremely long (like the one from RA3 to ICA2) I don't really want to continue here without at least trying to fix what I don't like.

Originally posted by pacificblue
Do you really need two 5 V 1 A voltage regulators for <40 mA supply current? There are 100mA voltage regulators in surface mount and through-hole packages available.

That's actually a good one - I'm not sure actually, it just seemed natural to use the classics.

Originally posted by pacificblue

Why do you need six ground connectors with 10 pins each? If this PCB will be the star-ground, the connectors should be placed next to each other and next to the power supply terminal to keep the ground paths short.

That I cannot change, this connector is for interoperability with the driver board which I will buy from someone

Originally posted by pacificblue
Turn C1 and C2 by 180° and make the ground connection from top to bottom layer between them, instead of at the power terminal.

Will do, makes sense too. I just didn't think about it

Originally posted by pacificblue
It would look better, if you turned either ICA2 or ICB2 with all corresponding components by 180°. That is of course only for the symmetry, not for the function.

Ok, I'll try that;

I will suppose the layout of the chipamp is ok since I had no comments on it; which is a surprise.

Thank you
Philippe

[pacificblue]

The LME series is reported to be picky. If I were to use it, I would orient my first design in National's demo board and analyze, why certain things were done in a certain way on it. From there on go tweaking and optimizing the design for specific needs.
Decoupling and compensation are in the right place on your board and the entire power section goes to the connector, so there is little to comment upon.
A little more space between the LME and the connector would be good in case you need to add a heatsink.

[theAnonymous1]

A modern DAC can definitely be done with only two layers. I built a DAC with DIR9001/SRC4192/PCM1794A all on a 2-layer DIY PCB with a common ground plane. It performs flawlessly.