[dsavitsk]

Back from a short trip ...

Quote:

Originally Posted by Francis_Vaughan The point about the ground returns is interesting. In effect we are making the ground-plane the ground reference, and therefore we should probably take separate ground runs away from it for any connection. In effect the ground-plane is the centre of a star ground. So indeed, separate runs for the ground returns for the two separate power supplies.

Does this mean not connecting the grounds of the power supplies where they are, but instead conecting the ground of the TDA'a PS to the ground plane? Where would bea good spot for this?


Quote:

The trace to the HOST pin on the 2707 (the one run though the bottom left corner of the chip's pins) could actually be run from the other side of the pad, and then around the outside of the de-coupling cap for the pin next to it. This would enable you to get the de-coupling cap closer, which is always good.

there is no decoupling cap. It is a 1M resistor

Quote:

It also strikes me that there is no reason why a medium value inductor or ferrite could not be put in series with the HOST pin trace.

Done.

In fact, there are spots for inductors all around.

The screws are M4 size. The mechanical drawing of the screws shows an 8mm head diameter. In a pinch, I'll use a plastic washer.

So, other than the issue with the ground, I think this is about ready to go? Any more thoughts?

 

[tangent]

Out in that empty space to the left of the TDA chip, I'd drop an extra ground pad or two. Extra ground pads are frequently helpful, if only so you can stick a probe in one when measuring things. Make one of them big enough to accomodate a PCB-mount test point, if you like to use those.

 

[Francis_Vaughan]

Yeah, test points are always a good idea. It is bad enough pointing one probe into a mess like this without trying to balance two.

With the PS grounds, it rather brings to mind a general principle. I never like to have much air between a source and its return. Rather what we have been striving for in miniature, but here you have the supply to the 1543 miles from its ground return. I would always run the return as close to the supply as possible - just as a general principle. Currently there is a lot of loop area, which can never be good.

Otherwise it looks good.

 

[dsavitsk]

Quote:

Originally Posted by Francis_Vaughan here you have the supply to the 1543 miles from its ground return.

well, an inch or so anyway. At anyrate, everything is closer than had the PS beenbuilt on a seperate board.

Quote:

I would always run the return as close to the supply as possible - just as a general principle. Currently there is a lot of loop area, which can never be good.

Do you have a practical suggestion? I don't think that moving the second PS is really an option, and runnng its ground and connecting near the dac chip will involve a longer loop, and running under the transformer which I am imagining will induce noise.

 

[Francis_Vaughan]

By loop area I mean the area enclosed by the power feed and its ground return. The trick is to get the two traces close to one another. Heck, put them on opposite sides of the board and lay them over one another - although that is likely excessively obsessive. Only join the grounds on the ground-plane. I would not worry about problems shifting the trace slightly under the transformer outline. The outline is the plastic case, not the transformer proper. There is a very slight chance of picking up a bit of electrostaticly coupled noise from the windings, but not much. Currently you are picking up vastly more noise because of the large loop area picking up electromagnetic interference.

Some options.

If you were to find the space to drop the bridges down onto the same line as the caps, it all gets easy. The only thing stopping you is the location of the 7805, which seems to be needlessly pushed to the right, with lots of space to its left. Pull it left, get the parallel poly cap onto the ground-plane, and you have room to drop the bridges. Then the 100nF caps can drop too, and you have room for the ground return trace.

Just for completeness, you might like to extend the ground-plane under both bypass caps on the crystal. There is quite a bit of RF in those traces, so full ground-plane will help. Same goes for the power trace nearby, that should also be over ground-plane. There is no real need to cut the ground-plane back so agressively.

 

[dsavitsk]

I think the reason that the regulator is so far to the right was a concern to keep unregulated voltages as far from the pcm2707 as possible. If that is not a problem and the regulator can move to the left, should the ground connection from the dac ps follow the power trace and connect to the ground plane at the bypass cap in front of the 9V regulator?

 

[Francis_Vaughan]

That sounds fine.

 

[Francis_Vaughan]

I have one last (!) suggestion. Something that has been bugging me for a while. There is a general desire, certainly from some designers to avoid crossing digital signals and analog, and in principle that also means power supplies. There is a chance of some small amount of interference. What has concerned me is the power trace that runs across in the gap between the 2707 and 1543. The one that is currently run under the coupling resistors of the I2S connections. Any noise on this line might possibly add jitter to the bit clock. I had been puzzling about how to re-run this trace without causing grief. Then I noticed how it can be done.

If you take the right USB data trace, and run it between the two left pins of the USB connector you can get the trace onto the left side of the other USB trace - this frees up the space under the coupling resistor of the other USB data trace. Now you have a path to snake the power from the pad for the ferrite on the left side of the 2707 taking the 3.3v feed, allowing it to run under the various SMD devices and round to the power pin.

There is an argument that this might allow USB noise to couple into the power, but that would occur before the final ferrite and de-coupling cap, and will be vastly less intrusive than any coupling onto the bit clock line.

 

[Francis_Vaughan]

OK, wasn't the last. I can't quite tell, but it looks as if there is a mistake in the 3.3v feed to the top right of the 2707, the power goes through two SMD components in series. One assumes that the second component is a bypass capacitor, in which case the trace from the first SMD component goes to the wrong pin, and the other side needs a via to ground.

Also, wherever you can, try to slide the bypass caps as close to the power pin they server as you can. There is scope for a little jiggling about in a few places. As a general principle the via to ground on the other side of the de-coupling should go as close to the corresponding ground pin on the chip as it can.

 

[dsavitsk]

Quote:

Originally Posted by Francis_Vaughan I have one last (!) suggestion.

It seemed easier to just run it on the outside. The USB jack's pins are really close, and I'd rather not try to get in there.

Other changes are the already discussed ground change. I also added some diagnostic ground pads, and a pad by the 120uF cap so a larger cap can be used. Oh, and I also moved the N pad back, but spaced it for a terminal block and added pads for a bypass/film cap on the output.

Quote:

I can't quite tell, but it looks as if there is a mistake in the 3.3v feed to the top right of the 2707.

It is a pullup resistor (and an inductor) to the DT pin.

Here are the changes:

 

[Francis_Vaughan]

Well I'm out of ideas

I say print it!

 

[steinchen]

just a small and minor note: the trace from the 1M resistor to the choke could be routed through the center of the upper two pads of the choke for maximum clearance

and a question to the wiring of the transformer's primary pins: aren't there drawbacks due to the paralleled traces and the 90° crossing of the blue trace from the right most pin ? I'd put the blue trace two points south.

 

[dsavitsk]

Boards are ordered. I made a small change at the end which is that the smoothing caps I had chosen were too tall for the case. In order to get them shorter without resorting to less capacitance, I had to move up to a fatter cap (the 1800uF/25V fm short version.) This required moving the 7805 and associated stuff more to the left. Hopefully not a big deal

Quote:

Originally Posted by Francis_Vaughan Well I'm out of ideas I say print it!

Thanks very much for all your help. I'll post some pics, etc. once they are here.

Quote:

Originally Posted by steinchen just a small and minor note: the trace from the 1M resistor to the choke could be routed through the center of the upper two pads of the choke for maximum clearance and a question to the wiring of the transformer's primary pins: aren't there drawbacks due to the paralleled traces and the 90° crossing of the blue trace from the right most pin ? I'd put the blue trace two points south.

I moved these about a little to add a bit of clearance. The 90 degree cross is going to have to remain, so hopefully it isn't a big isue.

 

[frdchang]

hey,

if you have an extra board, i will like to populate one as well since i am in need of a usb dac and like my non-os dac sound. (1543 as well).

so name a fair price and shipping and i can mail you a check or paypal whatnot.

or can you post your expresspcb files for those that want to purchase their own boards? (it is great that you made everything fit in their mini board service)

frdchang@berkeley.edu

 

[dsavitsk]

For now, I won't have any extra boards. However, I will get the board files online sooner than later. Check my website (http://diyaudio.ecp.cc) for board files, parts list, directions, etc. -- probably within a week or two.