[cobaltmute]

Okay, I was taking some of the link as gospel so I did a quick test in sim:
 

 
V1 = 12V AC rms
D1, D2 = 3N254
C1, C2 = 100uF
R3, R4 (load resistors) = 499 Ohms, just because that is what came up when I went to add them to the schematic
R1 = 0.5 Ohms
Oscilloscope test points are the top of the C's.  Top trace is R1, Bottom is R2
 
I played with R2, varying from 5 to 100 Ohms.  100 Ohms is what is pictured chosen for it very evident effect.  Putting 100R in line is not what I'm planning on doing for dissipation and voltage drop reasons.  Increasing the value of R between the bridge and the capacitor does smooth the waveform in all cases I tested.  It seemed that the turn on "spike" occurred over a "longer" duration in time creating a smoother waveform.
 
I also tried adding bypass caps to the bridge in the sim, which didn't appear to do anything.
 
Feel free to sim and rip apart anything I just said.  I know well enough that sims and my methodology can be wrong
 

 

[00940]

 
Quote:

I also tried adding bypass caps to the bridge in the sim, which didn't appear to do anything.
 

Don't worry, it's probably due to the limits of the diodes' model in spice

 

[cobaltmute]

Quote:

Try moving the AC input to the left board edge, then the diode bridge just inward from that but rotated 90 deg CCW, then R3. R3 might not have to be that big. It should only have a big V drop across it while C3 is charging up. You might be able to specify a wirewound or other surge-tolerant resistor type here in order to get away with a wattage rating closer to normal operating conditions.

 
I've moved this to a vertical resistor in the next revision (to be posted shortly).  I've also made sure that the hole spacing is spaced large enough that you could use a TO-220 power resistor there (but you may have to bend it out from C3 a bit to fit)
Quote:

 
If you can't talk yourself into making enough room for AC input screw terminals, at least make the pads big enough to accept 18 ga wire. They could probably only take 22 ga at the moment.

 
With the vertical R3, I've added the bigger terminal block, but the holes were 1.4mm in diameter and 18ga is 1.02 so it should have been good the way it was.
Quote:

 
The bridge snubber caps might lay out a little straighter if you stagger them to both sides of the bridge in addition to both sides of the board.

 
Like to know you feelings on the next revision, but I'm not sure what was wrong with what I had done.
Quote:

 
You have several broken fenestrations. Decreasing the trace width can help here; keep in mind that 4 x 10 mil is still 40 mil total, and it's over a short distance, so narrow trace widths don't hurt as much as what you'd normally consider a trace. If you absolutely can't get a plane to completely enclose a pin enough to give 4 connections to the plane, move the plane edge back toward the pin so you get only 2 or 3 clean connections; make the tiny 4th connection stub go away.
 

 
This was Ultiboard messing with me.  I had to re-pour the copper areas to fix this as I would tell it to make them smaller, but wouldn't do it.  All of them are 10 mil now.
Quote:

 
The middle plane bottom edge can come up away from R7. It's doing no good pushed down that far.
 

 
Done
Quote:

I'm not sure the left plane does much at all. Going back to a single thick (~100 mil) trace here that runs around the left and top edges of the board would be just as good. It's okay to neck the trace down to pass behind Q3.

 
I was looking at that and I've agreed.  I did it as a plane rather then a trace as Ultiboard wouldn't add thermal relief on the trace.
Quote:

 
C4: you've made a dual cap footprint here? I'd try to share the negative pin between them.

Yes, there is two footprints here.  8mm, 3.5mmLS and 10mm, 5mmLS.  Love to share the negative pad, but the part fit is extremely tight at the moment to both the op-amp and the other resistors.
 

 

[cobaltmute]

Rev 0.23
 
- R3 is now vertical and can be spec'ed at a TO-126/220 power resistor
- moved the bridge up to fit the terminal blocks.  Also made the + and - holes of the bridge larger to accept 18ga wire direct if you want to use to board as a straight DC regulator.
- various changes as noted by tangent.
 
Full PCB:

 
Bottom Ground Plane:

 
And just so that all can see perspective, 100% scale stuffing guide:
http://dl.dropbox.com/u/630887/r1-r0.23-stuffing%20guide.pdf
 
Feeling pretty good about this at the moment.  The only real thing that I feel is an outstanding item is remote sensing.  Going to SMT in the reference and feedback section, I know I could make it fit, but I'm not ready to go there, yet.
 
I'll start working on a BOM for y'all to tear apart.

 

[tangent]

Quote:

I also tried adding bypass caps to the bridge in the sim, which didn't appear to do anything.

 
Ideal, perfectly-matched diodes don't need snubbing. Real ones do.
 
Snubber caps are a poor-man's way to get some of the benefit you see people going for when they use exotic diodes in a bridge. (HEXFREDs and such.) A lot of the benefit is in lower RFI, rather than things like reduced noise that you'd see in a simulator.
 
 
Quote:

Like to know you feelings on the next revision, but I'm not sure what was wrong with what I had done.

 
I was just thinking that you could probably make the traces from the bridge pads to the cap pads straight.
 
Another thing I thought of later is that you could make dual SMT/thru-hole footprints if you can get away from caps on opposite sides of the board.
 
 
Quote:

Love to share the negative pad, but the part fit is extremely tight

 
You could probably do it by making a custom part with 3 pins. In EAGLE, when you do this, the result has to be routed very carefully unless you give the schematic symbol 3 pins, too and hook them up in the schematic correctly. Dunno how elegantly Ultiboard would handle such a Frankenpart.
 
 
Quote:

R3 is now vertical

 
I don't know your C3 diameter, but if it has the same pin spacing as the next size larger up, some might want to take advantage of the space you have around most of C3. You'll need to move R3 down a bit to make room for a larger cap.
 
You might add a silkscreen circle for the larger cap diameter as a visual keep-out boundary.
 
Lookin' spiffy, Erik!

 

[rds]

Did you intend to have the ground plane extend half way under the op-amp?

 

[cobaltmute]

Quote:

Did you intend to have the ground plane extend half way under the op-amp?

Yes, and the logic for that is earlier in the thread.
 

 

[cobaltmute]

Quote:

You could probably do it by making a custom part with 3 pins. In EAGLE, when you do this, the result has to be routed very carefully unless you give the schematic symbol 3 pins, too and hook them up in the schematic correctly. Dunno how elegantly Ultiboard would handle such a Frankenpart.  

 
I just did the Frankenpart thing and didn't like how it turned out. So I ultimately just said screw it and am going to use the bigger part. It hangs off the board by about a 1mm or so, but it's easier this way
 
Quote:

I don't know your C3 diameter, but if it has the same pin spacing as the next size larger up, some might want to take advantage of the space you have around most of C3. You'll need to move R3 down a bit to make room for a larger cap.
 
You might add a silkscreen circle for the larger cap diameter as a visual keep-out boundary.

 
The cap was a 16mm, 7.5mmLS. I've changed it over to a 18mm, 7.5mmLS. Little pushing around but it still fits.
 
Quote:

Lookin' spiffy, Erik!

In no particular order, there is a lot of credit for this to yourself, 00940 and rds.  The layout is significantly better due to the feedback from all of you.  I really, really appreciate it.  I'm amazed at how much has ended up on this small board.
 
I'll post the next revision in the morning.  Too tired/lazy to take the screen caps now.

 

[tangent]

Quote:

Did you intend to have the ground plane extend half way under the op-amp?

Based on 15 minutes of datasheet diving, it's probably fine.
 
The question is, are pins 5 and 8 high-impedance inputs? The answer is, "maybe".
 
The canonical chip for this regulator is the AD825, which says these pins aren't connected to anything on the die. Several other common AD chips are this way, too. All of these should be fine with the plane capacitance.
 
Many chips use these pins for output offset nulling. Only two of the datasheets I looked at even give a schematic for this, and only one of them gave part values. The pins connect to resistors in both cases, and they were on the order of 10 kΩ in the schematic that gave values. It seems a sensible value range for the other schematic, too, even though the nulling circuit differed. This probably isn't high enough impedance to be a problem.
 
The AD797 is also a common chip in this regulator, and it uses pin 8 for a "decompensation and distortion cancellation" feature. There is no internal schematic given, but the description for the feature makes it clear that it lets you modify the behavior of the feedback loop. That does suggest that it might be a high-impedance node in the internal circuit.
 
As I see it, Erik, you have two choices: 1) maintain a list of op-amps known to work and warn people off of rolling unless they have a scope; or 2) pull that plane back. Personally, I'd cut the peninsula under U1 off entirely and put the bypass cap in parallel with R1. It's only the V+ end that needs to be close to the op-amp.

 

[cobaltmute]

Okay, I get it.
 
Rev 0.26
- Moved R5 and R6 apart to be on 0.1 spacing to allow the use of a DIP-4 socket
- C3 footprint has been changed from 16mm to 18mm, both 7.5mmLS.  This allows a larger cap in the same space on the board.  However an 18mm capacitor will not work with the heatsink over the board.
- C4 has been changed to a 10mm, 5mmLS cap from a 8mm, 3.5mmLS cap.  Easier layout and allows for low leakage options with 5V references.  It does however hang off the board slightly.
- Ground plane has been rearranged.
 
One change that I want opinions on is the bypass caps around the bridge.  I moved both caps that go to the + rail to the same side of the bridge.  I was worried about clearances under the board with standoffs.  Anyone have any opinions if it is good or bad?
 
Aside from the question about the bypass caps, I think the PCB layout is pretty much "fixed"
 
3D View:

 
PCB:

 
Bottom layer:

 
Stuffing guide (at 100% scale)
http://dl.dropbox.com/u/630887/r1-r0.26-stuffing%20guide.pdf

 

[tangent]

Quote:

One change that I want opinions on is the bypass caps around the bridge.  I moved both caps that go to the + rail to the same side of the bridge.  I was worried about clearances under the board with standoffs.  Anyone have any opinions if it is good or bad?

Seems fine to me.
 
I'd add circles for the screw head and standoffs as keep-out markers. You could do it on the silkscreen layer, but I think I'd put them on a separate layer not used for the Gerbers, if Ultiboard can do that.
 
You might look in your part library for mounting holes that include these features. In EAGLE, some parts do have these circles, some don't.
 
One more nit: the left Q2 pin has an incomplete fenestration.
 
I like how you've chamfered the planes to allow more clearance between the unregulated and control grounds.

 

[rds]

Looking really good!
 
I'm wondering if you have enough space for a heatsink on Q1 that faces in towards the board?
Also personally I'd like to see a little more space between R3 and C3.  Having things that generate a lot of heat potentially touching the electrolytic capacitor could shorten the useful life of the power supply.
 
As for the diode caps, you want the trace between the source of transients and the cap as low impedance (or short) as possible ...though I do agree about the standoff issue.  How about having one cap topside between D2 and C3?

 

[cobaltmute]

@tangent:
 
Electronics Workbench doesn't carry the holes between schematic capture (Multisim) and PCB layout (Ultiboard).  You just add the hole separately in Ultiboard.  It is also treated as a unique entity that does not have silkscreen associated with it.  I do however mark my hole with trace clearances that are equal to screw head sizes.  As it is very easy to drop a plane in Ultiboard, I put on a plane and then layout parts so I'm clear of the hole.  I'm just worried about different size standoffs underneath. 
 
I knew you were going to pick on that on Q2.  I didn't want to pull the plane over more to cover it as I felt there wasn't enough space between the plane as it is.  I've now rotated Q2 90 degrees and it is fully in the ground plane.  As a side-effect, I've also been able to pull that plane a touch farther away from the un-regulated ground plane.
 
@rds:
If you use the 16mm cap for C3, the heatsink that tangent spec's on the TREAD should *just* fit.
 
For R3, I'm thinking the default spec will be a low value, something like 1 Ohm.  Not a lot of dissipation in that even if you're pulling 250ma through the regulator.  A 2 Ohm resistor equates 1/8W dissipation in R3 at 250ma, so I think we are okay.  So if you are really worried about heat from R3, there is two options:  1) Use a TO-220 power resistor, with heatsink away from the board or 2) skip R3 and short with a jumper. R3 may move down a bit as I play with the bypass caps on D2
 
As for the diode caps, being a bypass, I agree about the short trace portion.  I'll take another look at putting that cap on the top side.

 

[cobaltmute]

After being out of it for several days with the stomach flu, here is
 
Revision 0.27
- small layout change to fix the groundplane
 
I'm considering the PCB layout frozen.  It needs to be built and tested before any further changes.
 
Current schematic as PDF:
http://dl.dropbox.com/u/630887/r1-r0.27schematic.pdf
 
All Layers:

 
Bottom Layer:

 
And very importantly, for your consideration, a BOM:
http://dl.dropbox.com/u/630887/r1-r0.27-bom-a.xlsx
 
I've tried to choose what I thought were the best parts for each position.  I've separated the output dependent parts from the rest, as well as provided a few calculators for those that want to tweak their output voltages.
 
Let the critique of the BOM begin.
 
And while we discuss the BOM, it is probably a good time to consider ordering some prototype PCBs, so the question would be how many should I order?

 

[holland]

It's looking very sweet....will check out the bom in a few days, too much work to do and completely bogged down.