another jung super regulator pcb layout

[BrianGT]

Here is how I wanted to do power regulation on my dac:


I have a bunch of trace and ground planes removed in the picture.

Any reason that I should not do it like this?

The 5v is just for the dac chip, and the +/- 15 are just for the opamps. (will try using opa627 first)

--
Brian

[BrianGT]

Here is my pcm1792 layout, the top of the pcb, with the ground plane and all traces:



Note: I still need to add some vias, to increase the ground connections between the top and bottom ground planes, to optimize for shorter ground paths. (continuity)

--
Brian

[BrianGT]

Here is the bottom of the pcm1792 pcb:



I started working on the digital side now. Any suggestions for voltage regulators for the 3.3v digital? I have been considering the LT1793 .

--
Brian

[peranders]

Brian, you have made an excellent pcb.

One thing though.

I wasn't aware of that the preregulator is connected across the JG. This is surely a question for the experts (Fred?) but if you connect only 1k+ 1k//100uF(or something) across the series transistors, will not the JG get much lower impedance instead of the transistor alone (10-50 kohms)? I see the advantage but also that the JG doesn't work at it's top. This is just a thought. What does Jan say about this "impedance reduction"?

[peranders]

Brian, I think you should reconsider some traces. Very wide traces can make it hard to solder SMD parts. Choose wide traces where really need them.

[BrianGT]

Originally posted by peranders
Brian, I think you should reconsider some traces. Very wide traces can make it hard to solder SMD parts. Choose wide traces where really need them.

Which traces are you referring to? I made the power traces 40/60 and the signal traces are at 20.

--
Brian

[peranders]

You have 1206 or 0805 (can't see) and equally fat traces as the pads. This can be troublesome if you solder by hand. Sometimes you must have "hot relief" pads. This can be fixed with a fat main trace and them a 15 mil trace to the pad. Make this trace not too long (max 1-2 mm). The HF guys don't like it.

[peranders]

BTW: Shouldn't you use separate ground planes for the analogue and and digital section?

[Fred Dieckmann]

Originally posted by peranders
You have 1206 or 0805 (can't see) and equally fat traces as the pads. This can be troublesome if you solder by hand. Sometimes you must have "hot relief" pads. This can be fixed with a fat main trace and them a 15 mil trace to the pad. Make this trace not too long (max 1-2 mm). The HF guys don't like it.

Good advice, Brian. I see you have them on the pads into the ground plane. We call them thermal spokes where I worked. Even when oven soldering SMT parts will pull toward the larger thermal mass. Large pad size with respect to the trace will cause the surface tension of the melted solder paste between the part and pad to pull the part pretty squarely onto the pad when designed correctly. The parts come out straighter on the board after soldering than they were originally placed on the board by the pick and place machine. The correct consistency of the solder past after mixing is an truly an art. It has to be thin enough to go through tiny openings in the paste mask stencil correctly and thick enough to hold the part in place on the PCB during a trip trough several auto placement machines down a long conveyer belt (actually not a belt but a similar concept) and though a long convection oven with half a dozen temperature gradients. without the parts shifting significantly. I watched a woman quite good at mixing the solder paste before a run of my proto boards I was there to walk through. I told her she must be great at frosting cakes (the paste has almost the consistency of cake frosting). She was not amused! I'm sure her skill was the result of several years of manufacturing SMT boards. I learned to shut up after that when watching the very skilled labor involved in running an SMT line. It is a very demanding process to do right and requires a surprising amount of skilled labor for what one thinks of as an automated process.

[janneman]

Originally posted by BrianGT
Here is my pcm1792 layout, the top of the pcb, with the ground plane and all traces:



Note: I still need to add some vias, to increase the ground connections between the top and bottom ground planes, to optimize for shorter ground paths. (continuity)

--
Brian

Brian,

I am not familiar with your circuitry, but am I correct assuming that your board layout shows the analog circuitry on the bottom and the supply on the top part? If so, an immediate improvement in shorter lines, lower inductances etc would if you would have the analog stuff in the middle and the supply and other support cicuitry around it.

I know where you come from, but really these kind of PCBs need some planning ahead. This board I would start by making a rough layout for the analog part, moving from the middle outward. Then add supply stuff, again moving outward from center. Then add connectors, etc. Several times in between I would firm up the layout before adding the next ring. At the end you end up with something which is not nicely rectangular. I then do another round trying to shove things around to minimize board area without losing too much of the ideal layout. THEN I go out and buy an enclosure...

Jan Didden