Can you please have a look at my layout of pcm5102 dac?

michal_k

Well-known member
Joined
Nov 12, 2008
Messages
370
Location
France
Hi there,

It's first time I am doing a layout for a dac so I'd like to have you guys check out my pcb.

schematic for reference:
SCHEM.png


top layer:
TOP.png


bottom layer:
BOTTOM.png


Few comments/questions:
- I've chosen ADP151 for regulators. Is there anything better in terms of output ripple that one can buy in single quantities?
- Enable pins of the regulators are pulled up to the input voltage (hope it's the right way to do it) and are also available on the connectors so that turning off the whole module is possible by shorting them to ground.
- I've separated digital and analog grounds on the pcb and connected them in one spot. Not sure if it's helping, but if it's going to cause grounding problems please let me know ;) Also, charge pump is hooked up to the analog ground. I don't know how fast is it switching but maybe I'm not isolating high speed stuff from the analog part at all.
- Not sure how I should treat digital signals. I've tried to put as much ground plane between them as possible and use plenty of vias to form some sort of shield. Should I make the tracks of equal length?
- I didn't include output filter caps on the pcb cause they will be easy to solder on the output connectors and i don't know yet what kind of caps i want to use.
- The PCB is only 30x40mm so it should make a nice solution for a multi channel interface once the new xmos chips become available (I'm planning to use xs1-s as usb->i2s solution)

As always I am looking forward to your insights and comments.

Michal
 

Rochey

Well-known member
Joined
Jul 2, 2004
Messages
2,692
Location
Dallas, TX - Formerly UK
Thanks for designing in my baby.  :) (I defined the PCM5102 in my current role here at TI).

My few notes

- Consider one big ground - providing your layout is well segmented, you should be able to get away with it.
- Give yourself options to increase the value of the VNEG cap. (too big, and it won't charge, too little and it wont provide enough charge). 2.2uF is nice, but I've heard rumors that it may improve with a little more capacitance.
- XSMT is your friend. Use it through a pair of resistors to the 5V input pin. It'll mute the output before the regulators die etc.
- Consider adding a proper RC filter on the outputs, not just an R. (i see you added a note for this -- but add a footprint just in case for a 0805/0603 SMD cap)

That's all I have for now. I'll have more soon.

/R
 

millzners

Well-known member
Joined
May 7, 2010
Messages
219
I'd use one ground and not split them up, there isn't a lot of evidence to support splitting up grounds leading to less problems but I've personally seen problems as a result.

I would also click the option to remove untied ground plane, so you don't have those ground plane islands in there which aren't attached to anything.  You could drive a via through there if there's room.

Once you're completely done with the layout, it's a good idea to put ground vias through the entire remaining surface area in a grid pattern.  Just tie the two ground plains together as much as  you can, noting of course that most PCB manufacturers have a limit usually around 35 per sq. inch.

Check out the Micrel 5205 series regulators, just to compare.  I've had a lot of good designs use those.

That's all I've got for now.
 

gentlevoice1

Well-known member
Joined
Jan 14, 2008
Messages
126
Location
Aarhus, Denmark
Hi - a slightly "twisted" comment to your PCB: Some years ago an acquaintance of mine made some listening tests with identical circuits - the only difference was the thickness of the copper traces on the PCB board. He found that there were differences e.g. in terms of transparency, dynamics & immediacy when using thicker traces on the PCB. In my memory he ended up using a 135 umeter traces thicknesses which was the thickest he could get.

Regards,

Jesper
 

michal_k

Well-known member
Joined
Nov 12, 2008
Messages
370
Location
France
Thank you all for a helpful input. I've used your suggestions and here's the corrected layout:
ALL_REVA.png


[quote author=Rochey]Thanks for designing in my baby.  (I defined the PCM5102 in my current role here at TI).[/quote]
Yeah, I've read your thread on this forums and that's why I decided to check out this chip. You've pretty cool job over there. I'm checking out some graduate level jobs at TI but I'm not sure how to position myself to get close to the audio team and the kind of job you're doing.

[quote author=Rochey]Consider one big ground - providing your layout is well segmented, you should be able to get away with it.[/quote]
[quote author= millzners]I'd use one ground and not split them up, there isn't a lot of evidence to support splitting up grounds leading to less problems but I've personally seen problems as a result.[/quote]
done

[quote author=Rochey]Give yourself options to increase the value of the VNEG cap. (too big, and it won't charge, too little and it wont provide enough charge). 2.2uF is nice, but I've heard rumors that it may improve with a little more capacitance.[/quote]
I've added an extra pad for B size tantalum cap, that should give me a nice range of possible values

[quote author=Rochey]XSMT is your friend. Use it through a pair of resistors to the 5V input pin. It'll mute the output before the regulators die etc.[/quote]
I thought about it as well, but data sheet says that rise and fall times for xsmt signal should be less than 20ms. I have a 47uF cap in the psu which makes discharging it in this time hardly possible. That's why I've added an option to drive all control pins by an external controller, I presume I'll have a uC in this system anyway. Did I misunderstand the data sheet?

[quote author=Rochey]- Consider adding a proper RC filter on the outputs, not just an R. (i see you added a note for this -- but add a footprint just in case for a 0805/0603 SMD cap)[/quote]
done. Although it ruins my robo-face layout ;)

[quote author=millzners]I would also click the option to remove untied ground plane, so you don't have those ground plane islands in there which aren't attached to anything.  You could drive a via through there if there's room.

Once you're completely done with the layout, it's a good idea to put ground vias through the entire remaining surface area in a grid pattern.  Just tie the two ground plains together as much as  you can, noting of course that most PCB manufacturers have a limit usually around 35 per sq. inch.

Check out the Micrel 5205 series regulators, just to compare.  I've had a lot of good designs use those.[/quote]
Talking ground planes and stuff: when would I use ground plane on both sides of the pcb and when would using ground/Vcc planes be more suitable?
Thanks for suggesting micrel regulators. They look like a drop in replacement for adp's so I'll give them a go.


 

Rochey

Well-known member
Joined
Jul 2, 2004
Messages
2,692
Location
Dallas, TX - Formerly UK
michal_k said:
[quote author=Rochey]XSMT is your friend. Use it through a pair of resistors to the 5V input pin. It'll mute the output before the regulators die etc.
I thought about it as well, but data sheet says that rise and fall times for xsmt signal should be less than 20ms. I have a 47uF cap in the psu which makes discharging it in this time hardly possible. That's why I've added an option to drive all control pins by an external controller, I presume I'll have a uC in this system anyway. Did I misunderstand the data sheet?

[/quote]

The XSMT has two modes.
"Urgent Mute" - where a GPIO is controlling it
"System Power Loss" - where its monitoring an analog voltage.

There are two thresholds (I think it's 2.2V and 1.2V). If the voltage going to that pin shoots through those voltages quickly, then the device will assume a GPIO told it to mute. If it goes slowly, it assumes there's a real analog control voltage.

The rise and fall time issue is if you want a logic controlled mute. If the voltage drops slowly, the dac will attenuate the data digitally to begin with, then once it hits maximum attenuation, the device will do the analog mute.

/R
 

millzners

Well-known member
Joined
May 7, 2010
Messages
219
michal_k said:
Talking ground planes and stuff: when would I use ground plane on both sides of the pcb and when would using ground/Vcc planes be more suitable?
Thanks for suggesting micrel regulators. They look like a drop in replacement for adp's so I'll give them a go.

Ground plane on both sides seems obvious since you've got many components going to ground on either side, and really in any case where high speed edges is part of the design it's default to go with a ground fill on top and bottom (at least where I work).  Stitching everything together with vias just helps keep your grounds homogeneous.  Power planes are good for multilayer boards like 4 layers and up since you can burry the power in the middle and then drive vias directly to it instead of running power traces all over.  Functionally they're as good as ground planes for providing a DC reference plane for return currents to fast edge-rate signals.  However you typically want to avoid having power planes accessible to a wayward tweezer or some debris, so you usually want to keep them in the middle to avoid smoking something.
 
Top