[00940]

you would need a pcm2902, giving spdif, into a cs8416, giving I2S, into a cs4398. I wouldn't call it a clone though, even if parts are similar to the micro-dac, because the good choices for usb/spdif receivers are extremely limited and the power supplies, layout and so on matter a lot for dacs' sound, something you couldn't (and shouldn't) copy easily. You could of course substitute a WM8740 for example.

Another option is pcm2707 giving directly I2S to your cs4398 but then you don't have the possibility of a spdif input (coaxial or optical). It would be a bit stupid for a higher end dac.

 

[Alf]

Quote:

Originally Posted by diablo9 just curious, I heard Headroom Micro DAC use Cirrus CS4398, supposely a flagship part. Is there any reason not to use that?

CS4398-based DAC will be at least twice as big, will cost at least twice as much and what is more important it will not be PCM2702 DAC anymore

 

[MisterX]

lol.... when did that ever matter?

 

[Francis_Vaughan]

The important thing is that this is an evolutionary change to a known good design. With what one hopes are useful improvements to layout and PS, a body of experience can be built.

Doing such an evolution is more valuable than simply grabbing for the latest chip, and in a cargo cult design mentality doing a total scratch start.

 

[Botch]

Quote:

Originally Posted by Alf I replaced MAX1722 with TPS6734 and LM317A. Both ICs are cheap and easy to get. This gives us 9V from USB to power an amp. It will not be as good as TREAD but should do for portable use. Schematic v4

When reading this post I have assumed the LM317A is similar in noise and impedance behaviour to the larger 3 pin LM317T package.

A couple of questions/suggestions and something for everyone to read on power supplies:

- Looking at the schematic for the LM317A there should be a cap over R15 (between adj and gnd) as this reduces noise.
- Should we have 2 diodes (1 across the input/output & 1 across the output/R14) for protection it the case of the output voltage exceed in input voltage on shutdown, which could cause damage (maybe)?

Have a look on the datasheet for examples of this.

We also have to pay attention to the input and output caps for this regulator (ignoring 100nF caps). There is no large input cap and a 2 output caps currently - C25 (33uF) in parallel with C3 (1000uF). Not ideal at all, see the datasheet.

[edit] Oops, I missed seeing C20 (33uF) on the input but we still need to do something here as the output capacitance is far greater than then input capacitance.[/edit]

We need something before the regulator (let say ~1000uF) and a medium sized (lets say ~220uF) cap on the output. The output cap should have a medium ESR (not low ESR). What will adding a big cap on the input do to IC1 (TPS6734)? Need to check this guy also but guess it will be okay.

Why? I can try to explan badly but the easiest way it to have a read of these articles on TNT-Audio based on testing the LM117/317. The tests are based on the 3 pin version but should be applicable to the A version (similar technology I presume).

http://www.tnt-audio.com/clinica/solidstate.html

particularly:
http://www.tnt-audio.com/clinica/reg..._noise2_e.html

From this article:
"....bypass[ing] the adjustment pin, in our case with a 22uF ZL. And what happens? Noise is reduced tenfold with about 20dB."

and:
http://www.tnt-audio.com/clinica/reg...edance1_e.html

From this article:
"The output impedance of the LM317, even at DC, depends strongly on the load current, with impedance dropping with increasing load. This is not new, and it is precisely the reason why it is always recommended to ensure that such a regulator chip sources at least 10mA, preferrably 30mA, no matter what the actual load demands. At 100mA and more the impedance goes as low as 30mOhms or so, turning inductive above a low 400Hz. This is typical for a circuit relying on loop feedback, using an error amplifier with not a lot of gain and not a lot of bandwidth."

[OK, we have a load of ~40ma for our DAC and this is could be area where the 317T & 317A could behave differently (maybe), but is still important to think about it.]

and

"Adding an output capacitor effectively bypasses the regulator at higher frequencies. As the LM317 is inductive in these regions, this makes for a resonant circuit and hence some damping in the shape of a not-too-low capacitor ESR is called for: it is good to follow LM317s with a relatively big cap, but it is bad to use a low-Z cap there!"

[Need to do something about the status of the input and output caps.]

All the TNT Audio articles are worth reading as they have interesting info on different types of regulators.

Just my afternoon post for the group, back to work now. Lets keep the evolution of this design going.

Botch...

 

[diablo9]

Quote:

Originally Posted by Alf CS4398-based DAC will be at least twice as big, will cost at least twice as much and what is more important it will not be PCM2702 DAC anymore

hehe, that's OK, we can stick to PCM2702 this time, maybe next time someone will work out CS4398 design, in some distant future.

 

[Alf]

Good comment, Botch! I have updated the schematic. I also incorporated a few TREAD part selection hints from Tangent’s site. There are a few discrepancies between Tangent’s recommendations and those from tnt-audio. I wonder whether Tangent would care to comment this.

Schematic v5

Changes:
* Updated LM317 section.
* Implemented recommendations from the TI datasheet regarding REG102.
* Decoupled 5V and 3V3 sections. Now they both are powered from 9V as suggested by 00940.
* Sorted out the component names.

 

[Alf]

The last change has been quite a challenge. It took me about 20 hours to prepare this update. I hope the result is worth it.

Schematic v6

Board v4


Changes:
* Completely re-designed the board.
* Removed some ferrite beads – please comment if this makes any sense to you.
* Made wire pads bigger (Botch).
* Used a modified USB socket with pads around the holes for additional shielding and stability (Guzzler).

The part list has changed significantly. I aim to post a BOM draft tomorrow.

 

[doobooloo]

Looks great! This is definately very exciting - I'm looking forward to the test results!

 

[doobooloo]

One question... what's the purple line on the board layout that is feeding from the 5V pad to underneath the PCM2702 chip?

If this is just an external connecting wire that needs to be manually soldered, is it possible to:

1. Eliminate this wire completely; if this is not possible...
2. Have only one pad not three (connect the three pads on the board), and...
3. Have the pad somewhere in the open, not underneath the DAC...

OK so maybe it isn't a jumper wire...

Anyway, any input/enlightenment would be greatly appreciated!

 

[cetoole]

Quote:

Originally Posted by doobooloo One question... what's the purple line on the board layout that is feeding from the 5V pad to underneath the PCM2702 chip? If this is just an external connecting wire that needs to be manually soldered, is it possible to: 1. Eliminate this wire completely; if this is not possible... 2. Have only one pad not three (connect the three pads on the board), and... 3. Have the pad somewhere in the open, not underneath the DAC... OK so maybe it isn't a jumper wire... Anyway, any input/enlightenment would be greatly appreciated!

That looks like a trace on the bottom of the board to me. Great job Alf, that looks really sweet.

 

[Francis_Vaughan]

Umm, you are going to hate me, but I think you have seriously missed the point. Despite all the work put in, I'm afraid it is misdirected, and has taken the design in exactly the wrong direction.

You seem to be trying very hard to, in some sense, protect the analog supply rail, so much so that you have really badly damaged what was a good ground-plane. Indeed the ground-plane is almost destroyed and won't function properly. The thinking seems to be very much DC or audio frequency based, and has lost sight of the RF nature of the system.

The system will have harmonic switching components well into the hundreds of megahertz floating about. You must design the layout with this in mind.

Right, to the plot.

The analog power rail is not nearly so important as you think. Remember in all electronics it is symmetric, the ground terminal introduces exactly as much distortion or interference as the supply. But it gets worse. The ground is the reference supply, everything in the system needs an intact ground. We must manage the ground return currents, including those that flow between the digital and analog sides. The most important thing you must do in your design is ensure the integrity of the ground. This design has almost totally destroyed it.

The de-coupling of the power supply is a two terminal effort, that is why the functional units have brought out both power and ground, and very helpfully put them on adjacent pins. The best possible de-coupling of the power and ground is to short circuit the power and ground pins. Now, since that prevents the circuit from working we do the next best thing - we tie them together with a capacitor. That circuit between the pins must be as short as possible. If you look at the latest board you can find a number of examples where the power de-coupling has been forced to wend its way all over the place before connecting back to the relevant power pin. Trace out the path the current must take between any power pin and its ground pin via the de-coupling capacitor. Each of those paths is now an antenna, it will radiate or pick up energy from any nearby loop. You will find resonances and inter-component coupling that is rampant, leading to a very serious reduction in quality. The jitter will be very high, and the amount of energy coupling into the analog side from the digital side very high - so much so that the I/V converter will probably be well outside of its operational slew rate.

Look at the ground return path for the analog supply. Despite the lovely carefully laid out power trace, the ground return is left to its own devices to find its way home through a maze of little routes, and even the route to the ground pin of the regulator IC (and thus a route by which noise can be introduced) is very circuitous. Any energy coupling into this - and any disturbance of the ground will get straight into the analog side and produce distortion.

I'm sorry to say this, but the time invested has been wasted. There is nothing salvageable from this approach, and the board layout is vastly inferior to the previous version - which was pretty good, needing only some further pushing and tweaking to optimise.

 

[00940]

Francis : I've got a short question.

Does the PCM2702 really have to be put directly on the groundplane ? I designed the first version of this thing, the global layout of the beast is my fault

From what I remember, when trying first to put the groundplane on top, it was a real nightmare, mostly when trying to follow rules like "every digital line must be over a continuous groundplane".

 

[Alf]

Francis, I am a bit confused. You are talking about circuitous routes to the ground, while in fact the routes became much shorter with this layout.

Let’s have a look.

C19, C20, C21, C23 have the shortest possible direct routes to their ground pins.

C22, C24 have a bit more complex routes but shorter than before (C22 route goes under C24).

C18 - Not direct but quite short (under L5). I may be able to improve it though.

 

[Francis_Vaughan]

The idea is to get the critical traces and leads as close to the ground-plane as possible. The trick is to look at the system edge on. If you have the ground-plane on the other side all the ground pins must go to the ground-plane through a via - and so the loop area when viewed from the edge is much larger. When viewing the loop we include the lead-frame inside the package as well. These loops couple with one another. The bigger the area the greater the coupling.

The reason for running any digital line over a ground-plane is that the return current at these frequencies will try as much as possible to stay in that part of the ground-plane next to the line. There will be little current flowing elsewhere in the ground-plane. By cutting the ground-plane or moving the trace further away this effect reduces and the disturbance around the line increases. The same logic is true of the actual power supply lines between the de-coupling capacitor and the IC.

Luckily the adjacent power and ground pins help here - as opposed to those packages where the power enters and exits via opposite legs - which makes life much worse. But even with the gains due to these parallel power lines we must still cope with the remaining return currents for signals that move from unit to unit inside the IC, and at any instant these could be running from any power pin to any ground pin, so keeping the entire IC and lead-frame as close to the ground-plane is a good thing. Moving the ground plane from the opposite side to the near side reduces the distance from the plane to the traces dramatically, say 3 mm to much less than 1 mm.

By doing so we are able to keep the individual component systems in the IC operating with as low a disturbance as possible of their individual power. In particular with the least RF energy introduced from other parts of the system.

When the analog PLL for the DACs is so close to the other stages, and under certain circumstances there are close harmonic relationships between the different clocks (see later) there is significant danger of introducing signal correlated noise into the clock. This creates extremely unpleasant distortion products.

There is a special danger with inputs at 48kHz sample rate, as this will result in a 256fs = 12.288 MHz DAC clock, which is a bit close to 3/2 * 8 MHz - and there for a harmonic of the main system clock. So there is a possibility for some modulation products of particular worry to occur. Even more reason to keep the stages as clean as possible.