[Alf]

I updated the schematic and the board. It took me quite long time to implement all suggestions Francis made in his last post (keep them coming!). I re-shuffled nearly all components on the board making the layout more efficient. I hope I got it right this time!

Schematic v2
Board v3

Changes:
* New board size 50.5mm x 54mm. Now the board is 3mm shorter.
* Added a power switch (I guess it may be useful).
* Added C19.
* Moved the bypass capacitors closer to IC pins and rotated them. It is possible to move C10, C11, C14 a bit closer the board (~ 0.6mm) but not C13 and C12. The layout looked really ugly when I moved the capacitors. So I left them lined up.
* Optimized layout around the crystal and MAX1722.
* Many other minor changes.


I have been in contact with Maxim regarding MAX1722. They can supply me with any quantities (50+) of MAX1722. The bad news is that the final price including postage, taxes, and fees will be around 3.0-3.5 USD each. I may be able to bring the price down. I will keep you posted on this.

Now I am going to investigate potential replacements for MAX1722 and what can be used if the low voltage battery option is dropped. Any tips are welcome.

 

[doobooloo]

Ooh! Very interesting!

Makes me want to get back into DIY. I'll be watching this thread closely...

Thanks Alf!

 

[Sinbios]

Alf: if the USB power could be cleaned up to near the level of battery power, or even that of a nice power supply, then I'm all for it.

One thing, I think the original DAC wasn't bit-perfect -- is it possible to make this version bit-perfect?

 

[Botch]

Alf, you are doing a super job. And I'm sure you thought this was going to be a simple mod.

As for the MAX1722, I will probably not use them. I want to use the DAC for a desktop PC so will make a regulated power supply for it. (OK, maybe I'll get one MAX1722 in case I make a usb mobile version one day.)

Really minor point. Could you make the wire pads just a bit bigger? Seem to remember for the original they are a touch too small.

The oscillator is much cleaner. Could C15 & C16 be SMD parts? I'm not sure but it would give a little space so you could move IC3 to the left a bit, move C6 & C7 (rotate CW90°) down lower and make the 3.3V run shorter. Maybe C1 & C2 will have to move a little but there is lots of space up there. It a fun game.

Have a couple for Francis if he is still watching this thread.

Quote:

Originally Posted by Francis_Vaughan I notice that there is no seperate bypass capacitor for pins 2 and 4. Egads! Pin 2 is power for the clock generator. Junk on Vdd (pin 4) wil couple straight into the clock - jitter here we come. Get another capacitor right onto pin 2.

Francis, will the new layout clean this up enough?

Quote:

Originally Posted by Francis_Vaughan C18 will have to move, but that is no big deal, rotate it 90 degrees, and move the USB coupling resistors. You are going to end up with a transformer here anyway (trust me) so they are not important.

Can you explain this one a little more regarding a transformer.

Is looking good Alf. Keep the updates coming.

Botch...

 

[Francis_Vaughan]

It is looking much neater.

So a few more thoughts.

As Botch says, I wonder is a few, if not all the bypass caps might not be SMD. This should help the layout, and potentially improve performance. You can glue them to the back of the board then too, which may be a win if space gets grim.

The input transformer will, I think, be important - it gives you the freedom to get away from the vagaries USB power more easily if nothing else.

I think where I was trying to get to with the layout ideas is to look at the IC not as a monolithic thing, but as a system of connected units. The designers give you this ability since they bring out all the power pins. So if you refer to the block diagram in the data sheet it becomes clear what the goals are. Treat each of these units separately, give each its own well bypassed power so they can't interfere with one another, but also be cogniscent of the currents that must flow between the units, and thus the consequent return currents. Return currents are trivially dealt with with the solid ground-plane. It is hard to do better. So we worry about power. The digital power is in two places, clock and main digital logic. Each should be separately fed, and in this case this really means adding an appropriate ferrite bead isolator before each of the bypass capacitors. Thus split the pad C18 and C19 attach to, and feed each of the splits with an SMD ferrite bead.

Something similar might be appropriate for the analog side, although the lower frequencies involved might suggest some R in series with a bead as well, and perhaps more C.

You are building a mini LRC power supply filter for each unit - one designed to keep the crud floating about the board out of each unit. Since the units each have different functions we can design the filter to match the unit.

The exact choice of bypass capacitors should probably be revisited. The data sheet suggests significantly larger, but we must worry about series L. Guido provides some guidance on choice. There is much discussion on DIYAudio about this.

 

[Francis_Vaughan]

Groan, you are going to hate this one. It has been staring me in the face for ages, and it just didn't register.

The ground-plane is the wrong plane. That is: the component side should be the ground-plane. I kept thinking "why all these vias to ground" and then it hit me. I blame the antihistamines (spring here and the allergens are out in force.)

This is a lot of work to change. But if done means that most of the bypass capacitors can become SMD and be glued on without vias. Overall it will become massively cleaner and the RF performance improved further.

This does mean that to remain a reasonably clean layout quite a few components will swap to the other side, but that is, after all, part of the joy of proper double sided design. Some nice gains can be had. For instance you can drop R3 right under the crystal, improving the layout, reducing loop area further, and hauling back more space. Similarly you will see many more components that can swap sides and much that will tighten up. But much work.

 

[Botch]

Francis, I know that antihistamine blur.

I was having a similar thoughts on the ground plane but 100% wasn't sure about it.

Ideas at this stage:
- move the ground plane to the top layer.
- Change bypass caps to SMD's where appropriate.
- mount some components on the bottom layer when required (ie. for oscillator).
- add ferrite beads for the 3.3V digital supplies.
- look at 5V supply for VCC, VCCP, VCCR &VCCL (RCL for each one ?)

Can really clean up the over design but like you said, it's a lot of work.

Going to dig out the datasheet for the PCM2702 again tonight and have read up on the 5V supplies.

Alf, what do you think about all of this?

Botch...

 

[guzzler]

Just to put my little word in, changing the ground plane side should be a (fairly) trivial exercise, as Eagle will autoroute the ground plane around other traces. Just create a polygon and name in GND. Changing the bypassing to SMD is a good suggestion, as I feel that is the weakest part of the original design. I'm not a big fan of putting components under the board, I only did it on the PCM2902 layout (which I'm happy to share if anyone wants it) to squeeze in a little extra without making the board bigger. The best arrangement I've come up with for the oscilator would be this, with the components perpendicular to the osc:

CRC
|X|

Alf, in the CUSTOM.LBR library I sent you there should be a modified USB socket with pads around the hole. Connect these to ground and you get shielding of the plug and better mechanical stability

RCL for each 5V supply is not necessary, especially considering the quality of the REG102s. Also, remember the RCL network IS resonant, but damped (considerably) by the purely resistive element.

I don't have time to do much with this unfortunately, but best of luck and I will, of course, advise if requested

 

[Alf]

Quote:

Originally Posted by Botch And I'm sure you thought this was going to be a simple mod.

Yes, indeed. I guess it is not really Revision B anymore. It is now more of <b>The Ultimate PCM2702 USB DAC</b> Do you the sound of it? I do.

Quote:

Originally Posted by Botch Could you make the wire pads just a bit bigger? Seem to remember for the original they are a touch too small.

Do you mean the pads or the holes?

Quote:

Originally Posted by Francis_Vaughan This is a lot of work to change. But if done means that most of the bypass capacitors can become SMD and be glued on without vias. Overall it will become massively cleaner and the RF performance improved further. This does mean that to remain a reasonably clean layout quite a few components will swap to the other side, but that is, after all, part of the joy of proper double sided design. Some nice gains can be had. For instance you can drop R3 right under the crystal, improving the layout, reducing loop area further, and hauling back more space. Similarly you will see many more components that can swap sides and much that will tighten up. But much work.

I played with this a wee bit. My initial impression is favourable. The board looks much better. I will not be able to finish the new layout tonight though. Here are my additional ideas:
* C10, C11, C13, C14 may have to be 0805 package. It is pain to solder but this will give us a much better layout.
* R4, R5, R6 may need to go to the bottom layer.
* 5V may have to be routed to VCC and VCCR through the bottom layer.

Can we safely use a tantalum electrolytic capacitor for C12? A smaller package would help a lot.

Another related thought, since we go hardcore SMD, should we change all other capacitors to SMD too? Obviously CL, CR, C3, C9 will stay as they are. If we add more components to the board, the space will quickly become an issue.


Quote:

Originally Posted by Francis_Vaughan The digital power is in two places, clock and main digital logic. Each should be separately fed, and in this case this really means adding an appropriate ferrite bead isolator before each of the bypass capacitors. Thus split the pad C18 and C19 attach to, and feed each of the splits with an SMD ferrite bead.Something similar might be appropriate for the analog side, although the lower frequencies involved might suggest some R in series with a bead as well, and perhaps more C. You are building a mini LRC power supply filter for each unit - one designed to keep the crud floating about the board out of each unit. Since the units each have different functions we can design the filter to match the unit.

Quote:

Originally Posted by Botch - add ferrite beads for the 3.3V digital supplies. - look at 5V supply for VCC, VCCP, VCCR &VCCL (RCL for each one?)

I have some subconscious prejudice against excessive use of ferrite beads and RCL on a small board. I may be just completely wrong about it though. I need to think about it.

Quote:

Originally Posted by Guzzler RCL for each 5V supply is not necessary, especially considering the quality of the REG102s.

I am not questioning the quality of REG102s. However here is
RMAA comparison between battery and desktop PC USB made by Magsy for Revision A. It clearly shows that USB is not dealt with well enough. I think it is mostly because USB power is too noisy for REG102 to handle. Since we are moving towards powering the DAC and a paired amp from USB, this should be taken care of more efficiently.

Quote:

Originally Posted by Guzzler Alf, in the CUSTOM.LBR library I sent you there should be a modified USB socket with pads around the hole. Connect these to ground and you get shielding of the plug and better mechanical stability

Yep, I found it. Thanks.

 

[guzzler]

It's all relative on the USB power front; the noise level is still down at under -100dB, which is a figure any sound card would like to shout about. I do agree that the stereo crosstalk shows considerable variation (I don't know why), but is still down at -60dB. The distortion figures are actually better with USB, but the difference is much smaller there.

Makes sense to go all SMD, not much harder. 0805 is fine, just get small solder and a nice precise pair of tweezers (a pharmacy is a good place to try, Rapid also sell very nice ones)

I would very much recommend against R4,5,6 going on the other layer if you're going SMD. They are the primary input to the design, and therefore should be treated as delicate signals (which they are) and have no vias in them

 

[Alf]

Quote:

Originally Posted by guzzler It's all relative on the USB power front; the noise level is still down at under -100dB, which is a figure any sound card would like to shout about. I do agree that the stereo crosstalk shows considerable variation (I don't know why), but is still down at -60dB. The distortion figures are actually better with USB, but the difference is much smaller there.

I meant not enough for The Ultimate DAC

Quote:

Originally Posted by guzzler I would very much recommend against R4,5,6 going on the other layer if you're going SMD. They are the primary input to the design, and therefore should be treated as delicate signals (which they are) and have no vias in them

It is a digital signal. It should not be sensitive to such things.

Anyway I looked at the board again. It seems that I can avoid this.

 

[Francis_Vaughan]

A few more thoughts.

Again the trick may be to look at the functional block diagram, and also think about what sort of signals, clock rates and power supply requirements exist within. We do know a few things about how the device operates.

We have a 12 MHz ocsillator, this drives the spact USB logic. I am assuming that the 12 MHz does not get multiplied up - in the 2900 series chips it is, but they can use USB 1.1 and thus will need it. Since we are limited to USB 1.0 in the 2700 chips assuming 12MHz is probably safe.

The digital filter and DACs proper run at 128fs, so 5.6MHz. We can expect to see some energy at that frequency on the analog PS pins. We want to decouple these pins to avoid it getting back to other inputs. (Never forget - the decoupling of a power pin is just as much about stopping stuff getting out as it is about stopping stuff getting in. It is all about reducing coupling between circuits.)

So in the analog world we have 5 pins to worry about. 2 for the DACs, one for general analog stuff, one for the PLL, and one for decoupling the internal reference.

As good as any upstream regulator is, it is not residual noise from the regulator we are primarily worried about. It is the ability of the 2702's seperate components to interfere with one another. This is because the noise these components generate will have a high level of signal correlated energy. Energy from a DAC PS pin getting back into the PLL power pin will cause signal correlated jitter on the clock, and will create audible distortion components.

Although not directly connected to power, the reference pin does have a trace, and need a capacitor. We can assume that it is feeding the current reference in the DAC, and as the DAC element switches at 5.6MHz it will draw some current from this lead with this sort of frequency. The capacitor chosen will need very low ESR and ESL. It may be best to leave this part big enough to play with options to find the best type.

One thing we have no idea about is the PSRR of the 2702. TI are curiously mute on this subject, so we should assume the worst. We don't know the exact current draw into each component, which is a pity. But we can make some assumptions. The 5v supply is listed as having a max draw of 25mA. So since we have two DACs we might assume that each might draw a maximum of 10mA each. We could easily think of adding some 10s of Ohms of series resistance to decouple each DAC, and incorporate this R into a ferrite bead. Similarly for the PLL and general Vcc leg. The PLL could probably easily go up to 100 Ohms.

One could go on for quite a while. The option might be available to create an external clock - the 2702 will accept one. Then build a low jitter clock - for instance Elso Kwak's designs. They are not large. Once that was done one could think about a different DC-DC converter - one that can take an external sync, and then run the converter at a divided down DAC clock rate, avoiding the possibility of heterodyned image products appearing. And so it goes. But getting the PS and decoupling right will be a huge win.

 

[MASantos]

I think that all these changes look really promising but the board is already almost double of the original one. This design is supposed to be a portable one and if it gets any bigger than it's current size this will be a downside.

Alf, how big are those mounting holes??? They look around 5 mils in diameter?? I think that that is overkill, and something like 3 mils is more than enough( from the fisical point of view) . thsi owuld shave some space from the board!!

Manuel

 

[doobooloo]

Quote:

Originally Posted by MASantos This design is supposed to be a portable one...

Is it? If the design is to be portable I think it really should be DAC+amp on one board - which I would LOVE to see.

I think this is more like, transportable or just "small enough on a desk" concept... no?

Anyway. Personally I am fine with the bigger size (it's much better this way if I can use better components and it will fit in standard cases without creative mounting) actually but I can see the portability concern as well.

I honestly think someone should start an integrated usb dac + amp project soon.

 

[Alf]

Quote:

Originally Posted by MASantos I think that all these changes look really promising but the board is already almost double of the original one. This design is supposed to be a portable one and if it gets any bigger than it's current size this will be a downside.

The size of Rev A board is 1922 sq mm. The size of the new board is 2725 sq mm. The component areas are about the same size. The increase is caused by additional mounting holes and empty areas at the top and the bottom. The board is designed to fit the smallest Hammond and the empty areas are required to slide it in. It is still very portable and will be much easier to mount.

Now we have more components on the board and will have even more than that soon (RCL filters). However we will change more components to SMD and the final board may be even shorter than it is now.


Quote:

Originally Posted by MASantos Alf, how big are those mounting holes??? They look around 5 mils in diameter?? I think that that is overkill, and something like 3 mils is more than enough( from the fisical point of view) . thsi owuld shave some space from the board!!

The pads are 2.15mm in diameter and the holes are 1mm.