[tangent]

Quote:

But not getting what you mean when you say "pushed the AC entry to the far right".

 
He's observing that you're putting the noisy AC line in pads and the even noisier diode bridge right next to the high-impedance U2/Q5/U1+IN node. This will wreck your regulator's performance.
 
You want all the AC stuff to be shoved over entirely to one of the short board edges, and the high-impedance op-amp nodes and fully-regulated DC outputs over on the other. 00940's relayout helps, but I'd try to push the DC output connector clear to the left. Don't get caught up doing contortions to get this to single-sided. This is a high-performance regulator; don't nerf it.
 
You might even consider going 4-layer.

 

[cobaltmute]

I had this done before I saw tangent's comments.
 

 
My board has stayed the same size and I've managed to add a resistor before the filter cap.  Not totally happy with the ground trace, but the sensitive stuff is moved away from the bridge.  Now to think about moving that output around...

 

[00940]

Quote:

 
He's observing that you're putting the noisy AC line in pads and the even noisier diode bridge right next to the high-impedance U2/Q5/U1+IN node. This will wreck your regulator's performance.
 
You want all the AC stuff to be shoved over entirely to one of the short board edges, and the high-impedance op-amp nodes and fully-regulated DC outputs over on the other. 00940's relayout helps, but I'd try to push the DC output connector clear to the left. Don't get caught up doing contortions to get this to single-sided. This is a high-performance regulator; don't nerf it.
 
You might even consider going 4-layer.

Iirc, wasn't it you who observed how poor diode bridge placement wrecked the performance of the Velleman LM317 kit ?
 
I agree that pushing the DC ouput to the extreme left would be the best course of action. But there is maybe some more breathing room needed.
 
4 layers might be excessive though for an hobbyist design (especially using the opa134 ?). After all, Jung managed with one layer+screen (with some jumpers) and so did ALW. But they didn't have to deal with that nasty AC stuff.
 
 
 
@Cobaltmute: isn't there a capacitor in // with D1 lacking too ?
 
 

 

[cobaltmute]

Quote:

Iirc, wasn't it you who observed how poor diode bridge placement wrecked the performance of the Velleman LM317 kit ?
 
I agree that pushing the DC ouput to the extreme left would be the best course of action. But there is maybe some more breathing room needed.
 
4 layers might be excessive though for an hobbyist design (especially using the opa134 ?). After all, Jung managed with one layer+screen (with some jumpers) and so did ALW. But they didn't have to deal with that nasty AC stuff.
 
 
 
@Cobaltmute: isn't there a capacitor in // with D1 lacking too ?
 
 

Well that capacitor in parallel with D1 is there in some Jung schematics and not in others.  I'll have to look at it and see if it could fit.
 
The thing about pushing the output all the way to the left is handling the ground trace.  A bit more room would help, as would going to 4 layers.
 
I do have another op-amp in mind, but I'd have to switch to a SOIC layout to use it...
 

 

[rds]

Quote:

 
I do have another op-amp in mind, but I'd have to switch to a SOIC layout to use it...
 

It seems that SOIC would also allow you to move the output to the far left as well as optimize ground and power traces.  Might be a good solution considering that SOIC is very easy to solder.
 

 

[TheShaman]

Very interesting project!
Hope we see a bipolar version as well (and, dare I say, a group buy for boards as well!!).

 

[cobaltmute]

 
Quote:

Very interesting project!
Hope we see a bipolar version as well (and, dare I say, a group buy for boards as well!!).

You're not suggesting that I try to fit a bi-polar supply on that board are you?
 

 

[cobaltmute]

Since 00940 and tangent have brought it up (at least indirectly), here is my thoughts about performance.
 
Being on a TREAD sized board, the obvious comparison would be to the TREAD.  Going through the effort of building a discrete Jung regulator, I would definitely like to exceed the TREAD performance on noise specs.
 
Ideally, I'd like to be in the noise range of other Jung regulators.  Considering that it is a small board with rectifier on board, I don't know if that is obtainable, but that is my goal at this point.  I believe the schematic is sound and should give very good performance.  So for me, at the point, the challenge is to a) get an excellent board layout, and b) choose the right parts for that layout.
 
So I willing to hear all feedback.  Right now, I'm focusing on layout, then I'll have to optimize parts.

 

[TheShaman]

Quote:

 

You're not suggesting that I try to fit a bi-polar supply on that board are you?
 

Haha, nope!  

 
But even 1,5-2 times the size of the PCB would still be a very small high performance bipolar supply.

 

[tangent]

Yep, better now.
 
I'd thicken up those traces.  It doesn't take much IR drop to swamp ripple performance that's supposed to be in the -90 dB range if the regulator's working properly.
 
Re: 4-layers, I assumed there would be professional PCBs, even if only by group buy.

 

[cobaltmute]

Quote:

Originally Posted by tangent /img/forum/go_quote.gif
 
I'd thicken up those traces.  It doesn't take much IR drop to swamp ripple performance that's supposed to be in the -90 dB range if the regulator's working properly.
 
Re: 4-layers, I assumed there would be professional PCBs, even if only by group buy.

How thick are you talking about?  The thin traces are 15mil and the thick ones are 50mil.
 
I would assume professionally made boards as well.
 
As for 4-layer - the question that most strikes me is - what traces on what layers?
 

 

[cobaltmute]

Revision 0.11
 
- Moved the output block and appropriate re-layout
- Added the bypass cap on D1.
- switch to SMT op-amp
 
Again had this 99% done when I saw tangent's comments.
 

 
Not totally happy about the location of the ground test point and the LED, but couldn't figure out where else to put them. That said, I don't think I can get the voltage reference much further away from the bridge.

 

[00940]

I've got nothing nasty left to say 

 
One last little thing: provide for a bigger terminal at the AC entry point. You have easily room for a screw terminal.
 
 
 
PS/ That little discussion pushed me to this: http://www.head-fi.org/forum/thread/85561/post-pics-of-your-builds/7785#post_7318452

 

[rds]

Looks good.  How about a quasi ground plane on the backside?  Ultiboard (I think that's what you're using) can generate it with a couple clicks: http://web.alfredstate.edu/albaflr/Fall07/ELET7404/PROJECT%5CGnd-plane-ulti7.pdf
I agree on a terminal block for the AC as well.
 
Quote:

Revision 0.11
...

 

 

[cobaltmute]

 
Quote:

Looks good.  How about a quasi ground plane on the backside?  Ultiboard (I think that's what you're using) can generate it with a couple clicks: http://web.alfredstate.edu/albaflr/Fall07/ELET7404/PROJECT%5CGnd-plane-ulti7.pdf
I agree on a terminal block for the AC as well.
 

I agree on the terminal jack - I just need to make a footprint for one as Ultiboard doesn't seem to have a good one for a 5.08mm terminals.
 
I can do ground planes easy in Ultiboard.  I use them all the time to help place parts (as parts attached to nets don't get shoved during placement).
 
The issue I see with using a ground plane is how the current will flow from the output back to the bridge.
 
Here's what the board looks like with a bottom ground plane:

 
It gets cut badly but the traces for bootstrap.  Don't like it at all.  In a middle layer it might be okay, but we're still take dual layer at the moment.
 
The plane also messes up the "sense" portion of the reference and feedback to the op-amp.  However I could remove the plane around that part.