I guess I'll stick with the 2707. I actually think the tricky part is the D+ and D- pins as they are surrounded by pins that want 3.3v. as such, cutting the ground plane seems inevitable. I suppose that power traces could come from both sides, but this just creates a bunch of new problems.

Anyway, here is the latest incarnation. Monolithic bridges, I turned both the 2707 and the 1543 90 degrees to the right which made routing a bit easier. The connection to the ws pin of the dac goes up though the corner. The board manufacturer is going to need to adhere to some tight tolerances to get that one right, so hopefully it is okay. I also moved the DAC's PS around a bit to clean up some connections. There are still some cuts to the ground plane, but everything I tried to get rid of those caused more somewhere else. Any thoughts?

Good work, there. Now you need to start working on some of those clearances. Some places where I think you've got a potential problem:

- The traces going from the first primary past the second primary

- The dogleg trace going from the 1M resistor to the lower left pin of the filter choke. I'd turn the V going to the right resistor pad into a Y -- no need for "star" arrangements here. One leg of the Y will go down the middle of the filter choke between the pins, then dogleg over to the lower left pin at the last moment.

- Still not happy with the neutral AC input trace...

- The yellow trace on the right side of your monolithic bridges may be a problem, due to the proximilty of the SMT cap pads. There are simple rearrangements that will let you move this trace to the top layer. For instance, the blue trace from the left bridge to the big cap between the bridges could Y into the trace going to the big cap to the left of the leftmost bridge. Then the yellow trace I spoke of can come to the top layer. The other yellow trace can move to the top layer without any problems.

- The cap (?) hanging off pin 5 of the TDA1543 looks like it could rotate around and point downward without increasing the trace length between it and the IC. The thin traces running along the bottom edge of that IC would go between the pins of the cap. This will let you straighten the trace going to pin 6.

- I'd move those two ground pads in the upper left corner of the board to the left of the resistor bank, so you can align the resistors. Also, you can bring those resistors closer together; the outlines can overlap, and still allow the resistors to fit. This will make more space for bigger caps nearby.

- Have you run the thermal calculations on the 7809? It seems there's not enough room behind it to allow even a small heat sink to mount to its back.

OK, still a few things, and a bit of confusion.

Don't rotate the 1543. The idea was to get pins 1,2,3 right next to the 2707. Especially to get the bit clock trace as short as possible, and to avoid running the trace over any cuts in the ground plane. All else should subservient to these goals.

So, we can gain some space, and make some changes.

You could tweak the crystal oscillator layout a bit. There is no need to have the bypass capacitors share a via to ground. Split them apart and put them either side of the crystal. This will allow you to move the 2707 to the right a bit, which may make life a bit easier, but might not be worth the effort.

You have swapped the inputs to the DAC, somehow pins 1 (bit clock) and 2 (word select) have been swapped since your last layout. This will cause problems And has made the layout harder.

But, move the 1543 back over the 2707, and rotate it 90 degrees left to get the input pins as close to the 2707 as you can. Now we need to work on removing those cuts in the ground-plane. They are critical. Get the power from the left side of the chip not the right (except for the run to the pull up for DT which stays as it is.). The series resistors for the USB inputs can be moved so that they jump the power trace. (You may need to jump the USB to the ground-plane to jump one trace, but this is OK, especially if you do it well away from the 2707.) You can now remove all of the cuts in the ground-plane. If you are happy to run the data line thought a corner, take it through the top right corner, where it will run next to the other DAC inputs. You can punch the via to ground for pin 24 on the other side of the pin to make room.

You have the AGNDR and PGND sharing the same via to ground. Bad. In particular we want the PGND to go to the ground-plane with minimum distance. Vias have some inductance, and sharing the via with AGNDR means we may get some interference. You must split these onto separate vias. Integrity of the PLL power is paramount. Similarly, pins 25 and 26 should have individual vias to ground and not share traces.

The trace to HOST from USB power could be moved about. There is no reason to put the pull down resistor in a row with the other resistors. You have the entire trace gratuitously looped upward for no reason other than to put the resistors in a line. This further squashes things to the left needlessly, and has pulled the cut in the ground-plane under the 2707 where we really don't want it. With pins 1 and 31 no longer connected together, if you use vias on the outside of pins 1 and 31 you have room to slip the HOST trace out with no further ado. Putting the via on the outside of pin 1 is OK, even good, as it gets it right next to the other side of the de-coupling capacitor for the power input for that functional unit. Pin 31 couldn't care where its via is as we are not using the headphone amp in the chip.

A remaining possibility involves a small change to the schematic. Placing small inductors in series to control the rise time of the three DAC digital inputs. This technique is well accepted and seems to yield good results. Also, placing ferrites in series with the various +V pins on the 2707 can help to reduce local cross coupling. Although you are not using the DAC in the 2707, protecting the PLL, and keeping noise off the digital outputs remains crucial.

Quote:



That's pretty bad.

Quote:



My concern here is that since there is no solder mask on the board, and since the fuse holder is metal, I want to get the N pretty far away -- this was why the crazy routing before. I think I'll just move it to the other side of the mounting hole

Quote:



It looks like no more than a quarter watt even assuming the DAC is running full out and no v drop across the rectifier. Never the less, I'll leave enough space for a small clip-on.

Quote:



Ah, I see. Lots to do.

Quote:



What size inductor would you recommend? A side benefit is that they add a small space to route traces through.

Looking good.

Lots of spare space now
Space for an oversampling filter chip

Quote:



There are a couple of possibilities actually. Adding say a 100 Ohm resistor is probably a good thing. It will help to lower any residual circulating currents. In addition to the resistor a 1uH inductor in series could also be used. But I think just stick to the resistor for now.

Where you do need to add inductance is the +V inputs everywhere. A ferrite bead in series just before the decoupling cap is reached. This has the effect of isolating each of the sub-units from one another. Avoiding cross contamination of signals. Also adds lots of new routing possibilities.

Quote:



I am not too familiar with the design of dacs, but would it be possible to have an overampling space that is optional?
Or even a switch that could turn oversampling on and off?

Just a thought
-John

Quote:



Trivially. But both sides of the argument would regard the idea as a waste of time.

Me, I just like to poke fun every now and again.

Gotcha, thought I would just through it out.

It looks great dsavitsk!
-John

Quote:




What about those of us who are on neither side of the argument - but want to pick one. Such a switch would be *very* useful.

Quote:



Moving the DAC up a bit should create plenty of space for a SMD inductor, so there is probably no reason not to add it?

Quote:



Digikey wants me to choose filter frequency (either 50 or 100MHz), impedence (between 7 and 2700), and current for an 0805 sized ferrite bead. Any suggestions?

Quote:



I'm not sure that I'm on either of these sides. I'm on the side that says this could quickly get out of hand and never leave the design phase. Assuming that I can't be talked into adding it (and it depends upon difficulty of implementation as well as cost), I'll post the board files so if anyone wants to implement it they can.

By the way, I priced out the parts, and assuming you can find a TDA1543 it looks like it should come in at, or just under $50 + boards + output caps + whatever connectors you use. The board is sized for 4.7uF/50V N series blackgates, but I'll probably work in some pads such that using nice film caps, or at least a bypass, is an option.

Oh, you can also parallel DAC chips by stacking them and changing the values of the 3 1K resistors (though you may need to upspec the 8V regulator, and heatsink the 9V regulator, and it may stress the tranformer, and you would need to work in a fan ... but it is possible. I would guess that 2 chips in parallel is the limit.)

Much nicer, dsavitsk. Now you just need to get a little anal. You've got some pointless layer changes, and there are some traces showing stairstepping. For the latter, I believe you can double-click on a corner in EPCB to get its location; on those traces showing stairstepping, one of the ends of the trace will be very slightly off the grid.

Also, you should add some silkscreen circles around the mounting holes to match the size of the bolt heads you will be using. If you don't have a caliper, you now have a good excuse to get one. Even the cheap plastic ones you find at hardware stores will work fine here. Once you place those holes, you may find that you have to jigger some things around to avoid shorts to the case through the mounting bolts.

Another thing. I dont like that the 1543:s supply is tied to ground by the same trace as the digital.

Any ("digital") current flowing in that trace will modulate the analog supply.


Edit: One of the resistors beside the usb connector looks unconnected?

Quote:



Going by Guido Tent's guide, 100 Ohms at 100MHz is a minimum. If you can get it down to 50MHz probably even better.

Personally, if I was adding anything to the design the first step would be a better clock, and re-clocking, or alternatively, a better clock and a sample rate converter. I guess the entire philosophy behind NOS dacs would regard the idea of the sample rate converter as anathema (even though, like many of the justifications for NOS, it stems from a misapprehension about the mathematics.) But a very low jitter PPL and VCXO with re-clocking of the I2S would be a very valuable upgrade. I don't think it would fit easily. Close, but a big squeeze.

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.

There are a couple of slight tweaks in the layout that come to mind now.
The bypass capacitor for the 1543 could be pulled up slightly, so that its two pins are very close to the power and ground pins of the 1543. This would involve rotating the film cap in parallel with the regulator output out of the way, and juggling the other components a bit. In principle, the bypass cap should be as close to the pins as you can manage.

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. 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. Two good reasons. You can jump the power trace with it - losing the last cut in the ground-plane. But when in self powered mode the HOST pin only tells the 2707 when it is attached to a USB host. Just the presence of volts. No current. No signal. Adding a ferrite should remove another possible conduit for noise into the 2707. If it all ends in tears it could be replaced with a suitably low value resistor, but I feel a ferrite here is a good idea.