# A TREAD sized regulator - the r1



## cobaltmute

*EDIT: *Post 74 has a very much updated board for those that are looking for the latest info on the board, however there is a lot of good discussion in between that is worth reading about the revisions.
   
*Acknowledgments*:  Before I go any further, I want to acknowledge the work of Walt Jung.  Many portions of the regulator are based on publications of his on his website and without it, this wouldn't exist.  It also wouldn't exist without the work of Tangent and the publications of his on his website.
   
  For some reason, the two things that keeping seeming to capture my attention are DACs and regulators.  Don't know why, but they do.  Over the last year and a half, I've sim'ed many different variety of regulators as just an interest kind of thing.  During that time Tangent, for reasons that he has decided to keep private and I'm not going to pry, has decided to stop selling his regulators.  I've also seen during that time a few people lament the fact that the TREAD is no longer available.
   
  Well, I've decided to take a shot at building something TREAD sized.  For lack of a better name it is called the r1.  Unlike the TREAD, which is a LM317 based regulator, I figured a could build a Jung style regulator on the same size board.  The size of the tread was 5cm by 3cm.  My design, at the moment is 5cm by 3.3cm. 
   
  The basis of the regulator is taken from Walt Jung's 1997 article Regulator Excels In Noise and Line Rejection. With a few changes based upon other Walt Jung articles on constant current sources and buffered voltages references, the schematic was born:
   

   
  My board layout at current (green top traces, red bottom traces):

   
  At this moment, I looking for comments either on the schematic or the layout before I send it out for prototypes.  I'm hoping that the layout should be fairly low noise.
   
  I will post a few more comments on the layout soon, but being at work there is only so much I can post right now.


----------



## 00940

- Q6 is quite unnecessary, you could probably replace it by a resistor without losing any performance.
  - what's the point of R5, C3 ?
  - what are you using for U2 ? For U1 ?
  - the fat ground track in between the diode bridge and the output connector must be cut and replaced by a track starting at C2 ground. Nothing should be connected in between D2 and C2, it's your dirtiest ground.
  - Q5 really is wasted money, replace by resistor.
  - I don't like the fact that the sensing ground line is going under the very dirty (charging peaks) ground line linking the diodes bridge and the big cap.
  - If you don't mind being wasteful, a RC filter just after the diode bridge (something like 5-10 ohms before your first cap) quiet down the switching transients.
  - Decoupling for the opamp might not be necessary but might not be a bad idea either.
   
  Those things are touchy, best order a limited run of boards as a start.
   
  That would be for a start


----------



## holland

If you're going to add a CRC, see if you can add in a L as well, CLRC.
   
  what's your current output limit?  based on the pass transistor i presume.  also fixed voltage out?  one of the beauties of the lm317/lt108x circuits is some voltage adjustment.  A trimmer between r3 and ground?


----------



## 00940

Not CRC, RC


----------



## cobaltmute

Quote: 





00940 said:


> - Q6 is quite unnecessary, you could probably replace it by a resistor without losing any performance.
> - what's the point of R5, C3 ?
> - what are you using for U2 ? For U1 ?
> - the fat ground track in between the diode bridge and the output connector must be cut and replaced by a track starting at C2 ground. Nothing should be connected in between D2 and C2, it's your dirtiest ground.
> ...


 

 - Q6 - a resistor might work, but then again which is quieter? By designing for Q6, you can always build cheap with a resistor, but the other way around is harder.
  - R5,C3 - the dual resistor and cap combination is to reduce leakage current noise in the filter (taken from here: http://waltjung.org/PDFs/Build_Ultra_Low_Noise_Voltage_Reference.pdf and I've seen in a few other places as well)
  - U2 - LM336 (2.5V or 5V depending upon output requirement), U1 I've been simulating with a OPA134.  There is likely quieter choices out there.
  - Good point about the ground track, I can move that pretty easily.
  - True Q5 is wasteful, but I'm lazy about figuring out LED resistors and putting CCS is easy.  You can always put a vertical resistor there.
  - I'm not overly happy about the sense ground routing either, I could run it around the through-holes for the filter cap...
  - I'd considered the resistor between the bridge and the cap.  I've heard even 1 ohm can be very beneficial, but the issue is layout and size.
  - Looking at it now, I can see where I can fit a decoupling cap for the op-amp with not much issue so I'll put one in.
   
  Thanks for the feedback.


----------



## cobaltmute

Quote: 





holland said:


> If you're going to add a CRC, see if you can add in a L as well, CLRC.
> 
> what's your current output limit?  based on the pass transistor i presume.  also fixed voltage out?  one of the beauties of the lm317/lt108x circuits is some voltage adjustment.  A trimmer between r3 and ground?


 

 It is fixed out.  But the question I would ask is how ofter do you actually change voltage of a built supply?  I will take a look at sizing to put a trimmer there.  The other side of that though is that because the op-amp is powered from the regulated rail, some trim positions could end up in dis-functional regulator.
   
  As for current output, the limit would be CCS current of Q2 times by the hfe of the pass transistor.  I'm thinking of a J202 (Idss of 0.9 - 4.5ma) and a D44H11 as the pass (which looking at the curves seems to be about 125 as hfe).  So part selection determines the ultimate current limit.  The J202, could be replaced with J203 for higher limits.


----------



## holland

Quote: 





00940 said:


> Not CRC, RC


 


  Hehe, ok.  A common mode choke is still beneficial...and small with low DC impact.  SMD, on the underside...
   
  Here's one on digikey, from a quick search on smd chokes. http://www.tdk.co.jp/tefe02/e9713_acm.pdf
   
  Regulators tend to be less efficient as frequency rises, that is the ripple rejection is not as good.  By introducing a common mode choke, you increase the passive filtering as frequency rises, somewhat as compensation.  I like them.  YMMV.
   
  A small film cap at the transformer secondaries might be beneficial too, for hash coming in on the xformer secondaries.


----------



## 00940

Interesting read on C3, R5. I still kind of think that it's over-engineering in this case though. You'd make your life easier without those extra components. After all, the original Jung regulators didn't have those and still performed extremely well.
   
  With the currents you're considering, I'd completly drop Q4, as Jung did for his last version.
   
  Aren't you missing a cap in parallel with R2 ?
   
  And what about some protection diodes at the opamp input ?


----------



## holland

Quote: 





cobaltmute said:


> It is fixed out.  But the question I would ask is how ofter do you actually change voltage of a built supply?  I will take a look at sizing to put a trimmer there.  The other side of that though is that because the op-amp is powered from the regulated rail, some trim positions could end up in dis-functional regulator.
> 
> As for current output, the limit would be CCS current of Q2 times by the hfe of the pass transistor.  I'm thinking of a J202 (Idss of 0.9 - 4.5ma) and a D44H11 as the pass (which looking at the curves seems to be about 125 as hfe).  So part selection determines the ultimate current limit.  The J202, could be replaced with J203 for higher limits.


 
   
   
  How often depends on use.  For a tread, and dealing with opamps, sure, trying different voltages without any fanfare is pretty easy.  For tube heaters, same thing.  I understand this is a bit different, but voltages can be twiddled for DACs as well.
   
  It's hard to say.  Are you one to set a voltage and leave it, or are you one to try different voltages within tolerance.  Example, TDA1543.  What voltage there will also impact the standard passive I/V, but at the same time, you can try different voltages.  I think the same is true of the ESS DACs.
   
  You can size the trimmer so that it gives a small range of a couple of volts in the midrange of the opamp and within the transformer limits.
   
  You don't need to have it, it's just a nicety that some may like.  I've used both types of regulators, lm317/lt108x when I want some tweaking (opamp stuff, tube heaters, etc.) , and fixed like the 7815, S11, or S22 when I don't.


----------



## cobaltmute

Quote: 





00940 said:


> Interesting read on C3, R5. I still kind of think that it's over-engineering in this case though. You'd make your life easier without those extra components. After all, the original Jung regulators didn't have those and still performed extremely well.
> 
> With the currents you're considering, I'd completly drop Q4, as Jung did for his last version.
> 
> ...


 

 I did do a simple RC filter at first.  The issue at least in the early revisions was board space.  It was actually easier to do it this way with the extra parts from a space perspective.
   
  You are correct about the cap in parallel with R2 - don't know how I dropped that.
   
  I'd played with having the protection diodes there, and ended up removing them due to space/layout issues.
   
  Some of these issues could be quickly solved if I went to SMD parts (or a bigger board), but I wanted to keep this as through-hole for ease of building.


----------



## cobaltmute

Revision 0.8
   
  Changes based upon suggestions from 00940 and holland

 simplified the voltage reference filter
 changed the feedback resistor voltage divider with a trimpot for adjustability of the output voltage
 Add the capacitor on the feedback path
 Added decoupling capacitor for the op-amp using a SMT part on the bottom of the board
 dropped the BJT transistor from the bootstrap circuit
   
  Part numbering has changed to reflect the parts changes
  Schematic:

   
  Board:

   
  Thanks for the comments so far and keep them coming.


----------



## 00940

You're going to hate me in the end...
   
  Looking at your PCB, I've got the feeling that all the critical paths would be shorter and better protected if you pushed the AC entry to the far right (flipping C3 by 180°) and the output section to the middle.


----------



## cobaltmute

Quote: 





00940 said:


> You're going to hate me in the end...
> 
> Looking at your PCB, I've got the feeling that all the critical paths would be shorter and better protected if you pushed the AC entry to the far right (flipping C3 by 180°) and the output section to the middle.


 

 No hate - constructive criticism will never get hate from me.
   
  But not getting what you mean when you say "pushed the AC entry to the far right".  Do you mean along that edge or where the output is currently?


----------



## 00940

One of my class was cancelled today, so I had some time to kill at the library.

 Here's roughly what I meant:




 I really think it could be done single-sided, with just a pair of jumpers.This version is 4cm/6cm, quite a bit bigger than yours . Of course, Walt Jung had a grounplane on his versions, to act as a shield mostly.

 PS: I think you're under PCBexpress, so I didn't attach the eagle files. It's also not completly fool-proof and mistakes could maybe be found; I did it very quickly.


----------



## cobaltmute

Thanks for the layout suggestion.  You get your mind stuck on one perspective and sometime it takes some input from others.
   
  I'll play and see what you've inspired...


----------



## tangent

Quote: 





cobaltmute said:


> 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:


tangent said:


> 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: 





00940 said:


> 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.
> 
> ...


 

 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: 





cobaltmute said:


> 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: 





theshaman said:


> 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: 





cobaltmute said:


> 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: 





cobaltmute said:


> Revision 0.11
> ...


----------



## cobaltmute

Quote: 





rds said:


> 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.


----------



## holland

all the little traces with Q1, Q2, Q3, D1 and D6 can be moved top side.  If you reroute the topside trace between C1 and Q1 and C3.  Move the trace between C1 and Q1 going up along the edge after C1, and move the trace from C3 to Q1 lower between Q3/Q2 and Q1, which should shorten the trace between the + rail and Q3 as well.
   
  I'm also wondering if the ground plane should be cut between C3 and D2 using a smaller trace for ground between those 2.  I'm not sure, if the dirtiest ground is between C3 and D2, possibly restricting contamination may be beneficial.  I'm no expert though.
   
  BTW, there's more room, would you reconsider a common mode choke now that a SOIC package was introduced. 
	

	
	
		
		

		
			





  A small film cap on the AC input too? 
   
  Edit: also curious why the AC input traces are alternating sides?


----------



## rds

Yeah, it looks like all traces save maybe one could be moved topside and you'd have a near ideal ground plane.

     Quote:


holland said:


> all the little traces with Q1, Q2, Q3, D1 and D6 can be moved top side.  If ...


----------



## tangent

Quote: 





cobaltmute said:


> How thick are you talking about?  The thin traces are 15mil and the thick ones are 50mil.


 
   
  I like to get signal traces up to 40-50 mil if I can manage it on a given layout. That works well with standard 0.1" pin spacing components. Down around your SO-8 chip you'll have to neck things down a bit.
   
  As for the power traces, I design those heuristically. There is no one rule, and the rules I use often conflict so I have to balance them against each other. The ones that come immediately to mind are:
   
  - Prefer running major power and ground signals as planes rather than traces
   
  - When using traces instead, pick a size as large as possible on your board. Consider it the "bus width" in that particular design. There are a few such in the YJPS, for instance, over 100 mil. 150 maybe? That's probably too much for a board this compact. The point is, pick a size and stick to it. Use it only for those connections that can't be readily made with a plane, such as connecting two planes together.
   
  - AC side should be kept from DC side by at least 8mm. Use your CAD package's DRC rules to enforce this.
   
  - Keep space between unregulated and regulated DC sides.
   
  - Keep space around pads. Your board maker might be capable of 6/6 spacing, but that doesn't mean you need to push it that hard. I like to use more like 12-20 mil.
   
  - Use relatively thin trace widths for pours; 8-12 mll. This heuristic and the previous one combine to ensure that fenestrations do indeed improve solderability. Your current fenestrations are scarcely better than doing without because the four connections are so thick and the spacing so tight. That turns the plane into a big heat sink, increasing joint creation time and increasing the risk of cold joints and damaged components.
   
   
  Quote: 





> what traces on what layers?


 
   
  The first choice to make is whether you put the planes on the outer layers and the signals inside, or vice versa. The first choice is better for RF immunity and low-noise performance, while the second is better for DIY hackability. Another thing to consider is that the outer layers will have thicker copper. This tends to argue for putting the planes inside since they make up for thickness with area; let the outer layers get the benefit of thicker copper on the relatively thin traces.
   
  You probably want two layers dedicated to signals, one the primary signal layer, the other the "I need to jump this signal over that other one" layer. You use these like in 2-layer design.
   
  The other two layers are for planes. In old-school digital design, it was easy: one is +5V and the other GND. For this design, maybe they are unregulated ground and regulator ground instead. There should be no need for a +V plane, since the connection from the pass transistor emitter to the VOUT connector should be very short.
   
  Speaking of, that do-si-do you've got going on around Q1 bugs me. If you're set on the Q1 part, you can fix it by mirroring the design top-to-bottom so the Q1 emitter is on the left, and can thus be a tiny jump to the VOUT connector. An alternative would be to seek out a transistor with a different pinout to achieve the same end.
   
  Getting back to planes, you should split up your current single big plane. You don't want such a ready coupling path between the noisy AC and DC output sides, and probably want to segregate unreg and reg DC from each other, too. I would set up three grounds: UGND, CGND, and RGND. UGND is the unregulated ground, and connects all the grounds on the unregulated side of the board. CGND is the control ground; that is, for connections in the regulator proper. RGND is the regulated output ground, composed only of the GND pin on the VOUT connector and the output cap's ground. Each of these connects to its neighbor with a short, fat trace. Think of the separate planes as pools for current to swirl around in, not bothering the next pool down the line connected via a small stream.
   
  As for how this maps to layers, I'm actually having trouble justifying a fourth layer, but you're going to get it for free... All you need is one more layer for the two or three segregated ground planes. You don't want to put them on different planes because you're trying to avoid creating a coupling path. Maybe you just create a mirrored pair of each plane, to lower the overall impedance.


----------



## 00940

The design with the groundplane is somehow a step backward as it is now.
   
  Get rid of the ground plane for the power section. It's not really needed. Big fat tracks (power and ground on different layers and overlapping if possible) are more than good enough. Only keep a true groundplane for the interior of the blue square.
   
  You don't want a groundplane under the input pins of your opamp. You should move around the decoupling cap too, so that the pads aren't there either.
   
  The decoupling cap of the opamp could play tricks on the stability of the regulator btw; consider adding a small R in serie.
   
  On the tracks around the pass transistor, I'd at least put the output track on top of the board and the input one under the transistor. Less crossing that way.
   
p
   
   
   
   
   
  Here is the layout (except the top groundplane that was only shielding) on which Jung achieved outstanding performances.... just food for thought. Another point to consider before deciding how many layers to use is that you don't want to jump too quickly to production and you will need to do some testing. Prototyping runs with 4layers don't come cheap.


----------



## cobaltmute

Ok, Ok, I have learned my lesson - do not post a PCB design without taking a good look at.  I "poured and went".  Should have spent more time analyzing, but I was tired and was about to go to sleep.
   
  I'm working on a new, not ground plane layout, based on some of tangent's comments.  Should be easy to show with a ground plane as well.
   
  I'll post soon.


----------



## cobaltmute

Rev 0.15


 - Changed the CCS to a LED/BJT based one.  Why?  Went back and read the Jung article on CCSes.  The cascoded JFET is very good, but it needs lots of voltage to get that performance.  We're not likely to always have that, so it seemed that the LED/BJT would be better.
 - flipped the layout to straighten out routing around the pass transistor
 - bumped out some trace sizing.


 No, I haven't written off the request of the SMD choke, just focusing on other items at the moment.


 Schematic




 Board:



 Still need put a footprint in for 5.08mm screw terminals for the AC input, although 2.54mm terminals should fit.


 I'm also still looking at the ground plane.  I see the point of the screen that Jung/Didden did in the article referenced by 00940, but that was on a single layer design where the plane was only attached in one point to the circuit.  I don't have a good place to do that, but I can see that as a very valid item to do in going to four layers - one layer for the error amp circuits, one layer screen, and the other two layers split as ground.


----------



## tangent

Regarding the ground plane, I think you should put it back, enclosing just the regulator proper: from the board's top, right, and bottom edges to Q2 on the left. Then cut a hole around the op-amp.
   
  I'd increase the ground trace width between D2 pin 4 to just past the positive C3 pin as it nears the board edge. 100 mil at least.
   
  The schematic part labeled TPG1 is TP2 on the board?
   
  It may be an artifact of the imaging, but I don't see a via between the green op-amp pin 4 trace and the red tree ground. Is it missing, or just blown out in the picture?
   
  You might add a "+" silkscreen near the LED anodes. You can either modify the current footprints or just add text to the board. The current markings will be hard to discern once printed.
   
  I'd add some snubber caps around the bridge. Since you're already specing SMT caps for the op-amp, they'd work here, too.
   
  I don't see a reason for Q4. A resistor will work just fine, given that we have extreme confidence in our regulator, yes? That is, unless you were planning on making this a fully-adjustable supply with VR1, which I argue against below. With adjustment of a few volts for trimming, you don't need a separate CCS here.
   
  The same argument for Q5 is a lot harder to make. For one, it's not merely a LED current limiter. For another, the reference voltage accuracy directly affects the regulator accuracy; indeed, errors are multiplied by the op-amp gain.
   
  You want at least one resistor inline with VR1, maybe 2. Using a pot alone for gain adjustment will give too wide a range. You want a relatively small pot value here, with most of the feedback resistance in fixed resistors.
   
  I'd add an unregulated DC test point. Very useful in testing and debugging.
   
  Is the D2 footprint big enough? I would think a 1 or 2 A bridge would be wider than that. You've got enough room around it now for the size I'd expect, but you want the silkscreen outline to reserve all the space the part actually needs so you don't mess up and push something too close later.
   
  Q4 should rotate right 90°.


----------



## cobaltmute

Quote: 





tangent said:


> Regarding the ground plane, I think you should put it back, enclosing just the regulator proper: from the board's top, right, and bottom edges to Q2 on the left. Then cut a hole around the op-amp.
> 
> I'd increase the ground trace width between D2 pin 4 to just past the positive C3 pin as it nears the board edge. 100 mil at least.


 
   
  Next revision will have a ground plane, and we can discuss what how it is setup when I post.
  Quote: 





> The schematic part labeled TPG1 is TP2 on the board?
> 
> It may be an artifact of the imaging, but I don't see a via between the green op-amp pin 4 trace and the red tree ground. Is it missing, or just blown out in the picture?


 
  There is a via there, and yes, small label difference on the part - I'll fix that
  Quote: 





> You might add a "+" silkscreen near the LED anodes. You can either modify the current footprints or just add text to the board. The current markings will be hard to discern once printed.


 
  Take a look here at the grubDAC board - http://diyforums.org/GrubDAC/GrubDACboard.php.  The C pretty clearly marks the cathode, so I don't see a point in changing the silkscreen.  And we've seen no complaints from the grubDAC builders.
   
  Quote: 





> I'd add some snubber caps around the bridge. Since you're already specing SMT caps for the op-amp, they'd work here, too.


 
   
  I'll have to check space after I fix the bridge footprint (as noted below)
   
  Quote: 





> I don't see a reason for Q4. A resistor will work just fine, given that we have extreme confidence in our regulator, yes? That is, unless you were planning on making this a fully-adjustable supply with VR1, which I argue against below. With adjustment of a few volts for trimming, you don't need a separate CCS here.


 
   
  On the original layout Q4 made sense, as it was taking as much space as a resistor mounted vertical.  Now I've got space, so I'll put it as a resistor since it seems to offend.
   
  Quote: 





> The same argument for Q5 is a lot harder to make. For one, it's not merely a LED current limiter. For another, the reference voltage accuracy directly affects the regulator accuracy; indeed, errors are multiplied by the op-amp gain.


 
   
  Agreed and this will stay as is.
   
  Quote: 





> You want at least one resistor inline with VR1, maybe 2. Using a pot alone for gain adjustment will give too wide a range. You want a relatively small pot value here, with most of the feedback resistance in fixed resistors.


 
   
  I put in VR1 for adjustment, but I was never really sure about it.  I'm going to put it back to two resistor with no trim.  If you need an adjustable supply, you can socket your resistors.  Convenience or low noise is the way that I see the choice.
   
  I think part of this is the BOM as well - given that the noise is a result of referenence noise * gain, lower gain equals lower noise.  The best way to handle this is to spec parts based upon the desired output levels.  Easy enough to setup a spreadsheet with the parts choice for various output voltages (sort of like they did for this regulator: http://circulator.bravehost.com/Gminireg.htm )
   
  Quote: 





> I'd add an unregulated DC test point. Very useful in testing and debugging.


 
   
  Should be easy enough to add.
  Quote: 





> Is the D2 footprint big enough? I would think a 1 or 2 A bridge would be wider than that. You've got enough room around it now for the size I'd expect, but you want the silkscreen outline to reserve all the space the part actually needs so you don't mess up and push something too close later.


 
   
  Well, on check, you happen to be right.  Second time Multisim/Ultiboard has had a screwed up footprint in the master library.  And it is not just the outline - pin spacing is messed up too.
   
  I'll fix, re-layout and see what I can do about adding the bypass caps.
   
  Quote: 





> Q4 should rotate right 90°.


 
   
  No need to do so if I change it to a resistor.


----------



## 00940

I'd be curious to have measurements of a regulator with and without a jfet for Q5. Walt Jung didn't bother and all the guys who did PCBs didn't either (including Tangent at the time). But as you said, it's easy to fit a resistor in a jfet footprint.
   
  I'll wait for the final layout with groundplane for comments, Tangent nailed down all the problems I saw.  
   
  edit: I forgot that decoupling cap: seriously consider a resistor in serie with it. When I simulated a regulator in LTspice, I had serious oscillations if I had a "perfect" cap on the output.


----------



## cobaltmute

Quote: 





00940 said:


> I'd be curious to have measurements of a regulator with and without a jfet for Q5. Walt Jung didn't bother and all the guys who did PCBs didn't either (including Tangent at the time). But as you said, it's easy to fit a resistor in a jfet footprint.


 

 I should note that the part on the schematic shows a JFET, but that is not was it going there.  The part that is going there has the same pinout so it works as an excellent substitute.


----------



## cobaltmute

Rev 0.16 for your scrutiny
   
  Changes:
  - Q4 has been replaced by a resistor
  - Changed the test point naming and added an Unregulated test point.
  - Added a larger footprint option for the reference filter cap (noted on the schematic as C7).  This is needed to use 5mm LS caps.
  - Switched back to using 2 resistors instead of a trimpot for the feedback section.  I feel that this is more in line with the performance aspect of the regulator - you build it for a specific purpose.  You can always put the resistors in sockets if you want to build and adjustable regulator
  - Added bottom side ground plane.
  - Fixed the bridge footprint
   
  Still to do:
  - bypass caps on the bridge
  - screw terminals for the AC input
  - need to check space around Q1 to ensure a heatsink could sit over the board.  I believe it is close, it may just need to pushed right a touch.
   
  About the ground plane:
  There are two cuts in the plane to "break" it into three sections, Unregulated, Control and Reference.  The Unregulated section is for the bridge, the control section is for the bootstrap and the op-amp, and the reference section is for the voltage reference and the feedback loop.  I especially felt that it was important to not mix the reference section with the other sections.  Hopefully this layout works.
   
  I'd like the think that the PCB is getting very close to the time where a small test run should be made.  A baseline of its performance needs to be taken before trying to tweak it further.
   
  Schematic:

   
  PCB:

   
  And so it is more visible, bottom copper only:


----------



## 00940

It's  getting there indeed I think but:
   
  - The ground lead of Q2 should rather return to the unregulated groundplane (C3 groundlead) to keep the loop small and logical.
  - Your center groundplane can cover most of the opamp, just keep at bay from the input pins.
  - On the other hand, I would remove a strip from the center groundplane, removing it from under led2, Q2 and cutting it closer to the leftmost pins of led1, R7. Those components don't need it there and it would create a bigger gap in between the groundplane and the AC entry. If you tombstone R7, you can push led1 to the right a lot and increase the gap even further.
  - You shouldn't have a groundplane under the AC entry point and the diode bridge. It can only couple noise and do no good. At least cut away the bit around the ac entry and around the AC pins of the bridge.
  - I would bring R5, R6 closer to the opamp pin: flip C4 by 90° clockwise and they can go down a bit.
   
  Edit: I think you have room to implement remote sensing. You have to see if you want that feature or not. If you do, you have to link both the power supply and the ground to the sensing section by jumpers.


----------



## cobaltmute

Quote: 





00940 said:


> It's  getting there indeed I think but:


 
   
  Getting there also means that I need more explanations.  We're starting to get to the optimization stage and optimization without baseline is meaningless. 
  Quote: 





> - The ground lead of Q2 should rather return to the unregulated groundplane (C3 groundlead) to keep the loop small and logical.


 
   
  Looking at the both tangents and Jung's work, it seems that this path on the regulator goes to the the Control ground or directly to the central "star" ground.  There is small and logical versus putting the ground of this reference path to a noisier area of the board.
   
  Do you have any examples to show what kind of difference we could get by doing this?
   
  Quote: 





> - Your center groundplane can cover most of the opamp, just keep at bay from the input pins.


 
   
  Everything I've read about ground plane and op-amps suggests to remove it around the whole op-amp.  Now we are talking about slower op-amps for this purpose and the output has a very short trace to the first R, and we should benefit from the screen effect, while not affecting the op-amp too much, so I'll do this.
   
  Quote: 





> - On the other hand, I would remove a strip from the center groundplane, removing it from under led2, Q2 and cutting it closer to the leftmost pins of led1, R7. Those components don't need it there and it would create a bigger gap in between the groundplane and the AC entry. If you tombstone R7, you can push led1 to the right a lot and increase the gap even further.


 
  I'm going to make some further cuts/layout changes to increase the gaps, but on a small board it is tough.
  Quote: 





> - You shouldn't have a groundplane under the AC entry point and the diode bridge. It can only couple noise and do no good. At least cut away the bit around the ac entry and around the AC pins of the bridge.


 
   
  This makes sense, and will be done.
  Quote: 





> - I would bring R5, R6 closer to the opamp pin: flip C4 by 90° clockwise and they can go down a bit.


 
   
  They can only go down a fraction.  I'm spec'ing C4 to be up to 10mm/5mm LS.  The outline you see is the smaller 8mm/3.5mm option. 
   
  And I don't see the purpose in rotating C4.
  Quote: 





> Edit: I think you have room to implement remote sensing. You have to see if you want that feature or not. If you do, you have to link both the power supply and the ground to the sensing section by jumpers.


 
   
  Not a lot of room to do this.  But it would be a nice feature to have.  I'll see if it'll work


----------



## 00940

Quote: 





cobaltmute said:


> Looking at the both tangents and Jung's work, it seems that this path on the regulator goes to the the Control ground or directly to the central "star" ground.  There is small and logical versus putting the ground of this reference path to a noisier area of the board.


   
  In Jung's work ( http://waltjung.org/PDFs/Improved_PN_Regs.pdf , fig 1 and 3, same here : http://waltjung.org/PDFs/Regulator_Excels_In_Noise_and_Line_Rejection.pdf ) that goes to the input gnd (and he uses a looong track for that). Current goes back to C3 groundlead anyway, no reason to have it running all around the pass transistor. With the modulated opamp return ground currents passing by the same place, it isn't the quietest area of the board anyway.

   
  Quote: 





cobaltmute said:


> And I don't see the purpose in rotating C4.


 
   
  Brain fart... I don't know why I thought for one second that you had your opamp on the bottom side.  
	

	
	
		
		

		
		
	


	



   
  Stupid question.. don't you have enough room for putting back a DIP opamp ? To be in line with the through hole approach.


----------



## cobaltmute

On the second PDF you link to, it goes to the base of the op-amp in the schematic, but on the first link it does go to the base of the filter cap.
   
  I'm going to keep it where it is - for now.  I see this as a trade-off in where the return current is going versus the possible advantage of having a bit of screen under this portion of the board.
   
  As for moving back to DIP for the op-amp, it is possible.  However, given the fact that the op-amp I'm looking at is easier to get in SOIC versus DIP, I'm going to stay with SMT for the time being.


----------



## 00940

In the first link, it certainly goes to the input cap  
	

	
	
		
		

		
			




   
  You have a starground with C1 (input cap), R20 (Q2 for you), the opamp ground, going to a terminal labelled "unreg. gnd"


----------



## cobaltmute

Quote: 





00940 said:


> In the first link, it certainly goes to the input cap
> 
> 
> 
> ...


 
   
  Did I say that it goes anywhere other than to the input/filter cap in the first link?
   
  And in the first link, as you mentioned, on the PCB design, it runs all the way to the base of the input cap.  And if you look closely at the positive PCB layout, the op-amp return joins it right at the op-amp.
   
  This is why, in part, I think non-ground plane is better.  It is very clear on a non-ground plane board to see where the current goes.


----------



## 00940

Quote: 





cobaltmute said:


> Did I say that it goes anywhere other than to the input/filter cap in the first link?
> 
> And in the first link, as you mentioned, on the PCB design, it runs all the way to the base of the input cap.  And if you look closely at the positive PCB layout, the op-amp return joins it right at the op-amp.
> 
> This is why, in part, I think non-ground plane is better.  It is very clear on a non-ground plane board to see where the current goes.


 

 Excuse me then, I misunderstood you. Actually, there are no differences at all in between the two pdf. In both cases, the input cap, the opamp ground and your Q2 go to unregulated or raw gnd. *shrugs* Probably not very important, it's fairly constant current anyway since you're using a jft (or CRD ?). I promise I'll stop the nitpicking.
   
  Agreed on the groundplane thing


----------



## cobaltmute

Quote: 





00940 said:


> it's fairly constant current anyway since you're using a jft (or CRD ?). I promise I'll stop the nitpicking.


 

 Q2 and Q5 will be the same, which will be a depletion mode MOSFET.
   
  And nitpicking is important.  Especially when we are trying to chase the noise.
   
  Just at this moment, I think we should baseline the board, then nitpick some more.


----------



## rds

Quote: 





cobaltmute said:


> ...
> This is why, in part, I think non-ground plane is better.  It is very clear on a non-ground plane board to see where the current goes.


 


  On the other hand a ground plane provides shielding from environmental noise.  This may not have been a problem for Jung measuring in a controlled environment, but that won't be the case with DIY projects used in a home environment.


----------



## cobaltmute

I agree and that is why the board has a ground plane.
   
  But just dropping a plane on the board without thinking about layout and current flow will not get you low noise and may actually be worse.


----------



## rds

Quote: 





cobaltmute said:


> I agree and that is why the board has a ground plane.
> 
> But just dropping a plane on the board without thinking about layout and current flow will not get you low noise and may actually be worse.


 

  
  That you're thinking about the layout is assumed   But I would argue that given the parts are laid out in a reasonable order that simply dropping on a plane at the end without thinking about it would be an improvement (though obviously not recommended).  Of course "separating" the planes pre and post filtering would, intuitively, be better ...however, i've yet to see the FDTD sims to to suggest the degree of improvement or the optimum connecting strip impedance


----------



## cobaltmute

Rev 0.20
   
  - Tried to add the remote sense connections.  Didn't like what it was doing so removed them.
  - Tried to fit in screw terminals for the AC connection, see note below
  - Added bypass caps for the bridge
  - Update ground plane layout.  Re-routed some portions of the plane and changed the way that I was handling it to not have DRC issues.
   
  As for the screw terminals for the AC input, I'm having clearance issues.  As the board is right now, the 2.54mm terminals would hang off the board slightly, but they are only rated for 20 gauge at the largest.  I'd like to put the 5.08mm terminals, but it would push the bridge towards C3 quite a bit and require that R3 be mounted vertically.  Not sure if this would be the best, so open for opinions.
   
  All layers:

   
  Bottom Layer:


----------



## rds

I think a little overhang of the screw terminal could be ok if there is no other option.  Personally I don't have an issue with tombstoning R3 since C3 will already be quite tall.  Another option is to remove R3 - I'm not sure what function it's serving anyways.
   
  I think you forgot to cut away the ground plane under your op-amp.


----------



## cobaltmute

R3 does two things
  1 - it does provide an R-C filter to get rid of high frequency hash on the lines
  2 - It isolates the bridge from the big capacitor after it, which is said to improve the performance of the bridge.


----------



## rds

Quote: 





cobaltmute said:


> R3 does two things
> 1 - it does provide an R-C filter to get rid of high frequency hash on the lines
> 2 - It isolates the bridge from the big capacitor after it, which is said to improve the performance of the bridge.


 

 1 - So the claim is that the capacitor filters more effectively with a resistor in front of it?  I've never heard of this before ...do you know where this idea comes from?
  2 - This seems contrary to what isolation typically means.  Is this sourced from a datasheet?
   
  Sorry for the questions but this is a new concept for me that is counter intuitive to my understanding of electronics


----------



## 00940

@rds: http://www.diyhifi.org/forums/viewtopic.php?f=5&t=1707&sid=cc2526f67c0cce58a289430f41d2cb2c


----------



## cobaltmute

Quote: 





rds said:


> 1 - So the claim is that the capacitor filters more effectively with a resistor in front of it?  I've never heard of this before ...do you know where this idea comes from?
> 2 - This seems contrary to what isolation typically means.  Is this sourced from a datasheet?
> 
> Sorry for the questions but this is a new concept for me that is counter intuitive to my understanding of electronics


 
   
  Well, a capacitor to ground, C3, with a resistor preceding it, R3, makes a low pass filter.  I may be wrong, but that would improve filtering over C3 alone, at higher frequencies given the values that we will be dealing with.
   
  As for #2, 00940's link explains the item more correctly than I did.


----------



## tangent

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.
   
  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.
   
  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.
   
  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.
   
  The middle plane bottom edge can come up away from R7. It's doing no good pushed down that far.
   
  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.
   
  C4: you've made a dual cap footprint here? I'd try to share the negative pin between them.


----------



## rds

Quote: 





00940 said:


> @rds: http://www.diyhifi.org/forums/viewtopic.php?f=5&t=1707&sid=cc2526f67c0cce58a289430f41d2cb2c


 

 Thanks.  I found the argument in that thread too "hand-wavey" though.  I did find a textbook where the resistance was modeled, but that was in the case of line impedance and not intentionally adding resistance.  Anyways, I'll look into that more and leave this thread to the task of finalizing this very cool looking power supply.


----------



## 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: 





cobaltmute said:


> 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: 





tangent said:


> 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: 





cobaltmute said:


> 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: 





rds said:


> 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: 





tangent said:


> 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: 





rds said:


> 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: 





cobaltmute said:


> 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.


----------



## tomb

I'll build a couple.


----------



## c12mech

I would build a couple also.  All of your designs lately have been exactly the things I've been looking for.  I've been following this one from the beginning and have learned a lot just reading all the posts about the design process.


----------



## TheShaman

I'd be interested in a couple of PCBs as well.
  Unfortunately I don't have the parts to stuff them immediately, so it'd take me a while to order and receive parts.


----------



## Spacehead

2 for me then also


----------



## Avro_Arrow

If you have one left over I would build it too.
  Let everyone else have one first though.


----------



## cobaltmute

I still trying to decide how many to order, so you'll be able to get one Avro.


----------



## Avro_Arrow

Thanks, put me down for one.
   
  Quote: 





cobaltmute said:


> I still trying to decide how many to order, so you'll be able to get one Avro.


----------



## Yoga Flame

I'd like one too, but also cannot commit to building it anytime soon.


----------



## elliot42

I'm in the same position as Yoga Flame, I could buy one to build and test but can't say when I'd be able to actually build it.


----------



## Billyk

I'd happily build one or two. Don't have a scope though... So please consider me for two boards.


----------



## holland

one for proto, more for production runs (like 5 to 10).


----------



## rds

I can do some measurement if someone wants to send me a built proto, but won't be able to actually build one


----------



## cobaltmute

@rds: Given our proximity, I'll send you a proto (or two) to test.


----------



## cobaltmute

I have ordered the BOM parts so that I can test fit everything on paper to ensure that clearances are good before ordering the prototype PCBs.  I hope to have the PCBs ordered by the end of the week.


----------



## slowpogo

I've been following this and would love to get a board and build one, as well.


----------



## rds

Quote: 





cobaltmute said:


> @rds: Given our proximity, I'll send you a proto (or two) to test.


 


  sounds good


----------



## nullstring

I'll take one too. Sounds like the perfect PS for a budget/compact M^3.
   
   
  Colbaltmute, do you have any specifications as far as input voltage/output voltage, max difference between the two, etc.?


----------



## francisdemarte

Count me in for a proto too. I was a big fan of Tangent's THREAD.


----------



## cobaltmute

Just an update on the prototype PCBs:  I plan to put them on a panel with a number of personal PCBs and order them tomorrow.


----------



## cobaltmute

Quote: 





nullstring said:


> I'll take one too. Sounds like the perfect PS for a budget/compact M^3.
> 
> 
> Colbaltmute, do you have any specifications as far as input voltage/output voltage, max difference between the two, etc.?


 


  Input/output voltage difference really depends upon how much current you are going to pull through the regulator.
   
  In generic terms, the pass transistor has to drop the unregulated voltage to the regulated voltage.  Volts dropped times by the current is the watts of dissipation of the pass transistor.
   
  So you can have a high voltage differential at low current draw and low voltage differential at high draw and be in the same place.
   
  Ultimately, it depends on how hot you want to let the pass transistor get and how well you heatsink it.


----------



## nullstring

Sorry for mucking up your thread with rudimentary power supply stuff, but..
   
  Well, the other pieces of information I need to know is:

 How much voltage drop does there need to be to maintain regulation? (Sigma11 says something like 7V (or 9VAC before rectifier bridge)
 How many watts can a standard heatsink dissipate safely? I know this sort of a silly question because it really depends on the heatsink, but it'd be nice if someone could give me a ballpark.
   
  I have a transformer that outputs 38VAC when not loaded (not sure if that matters)
  And I think the powers supply needs to support 0.5 amps for M^3
   
  Assuming I need to drop 7V's to maintain regulation, thats 7*.5 = 3.5 watts...


----------



## cobaltmute

Quote: 





nullstring said:


> I have a transformer that outputs 38VAC when not loaded (not sure if that matters)
> And I think the powers supply needs to support 0.5 amps for M^3
> 
> Assuming I need to drop 7V's to maintain regulation, thats 7*.5 = 3.5 watts...


 

 The issue that I see here is that 38VAC through a full wave bridge = ~53V rectified. 
   
  First issue is the filter cap, C3.  BOM value is 63V, but you'd want to use 100V.  Haven't checked on what value is available here in a 7.5mm lead spacing in 18mm diameter, but it is likely small for the purpose.
   
  Second issue is that you are then dropping ~20V to get down to the point you will not blow the op-amps in the M^3.  That's 10 watts of dissipation.  You can pre-drop some in R3 with a power resistor and heatsink, but it seems high.


----------



## nullstring

Quote: 





cobaltmute said:


> The issue that I see here is that 38VAC through a full wave bridge = ~53V rectified.


 

 This is where I am a bit confused. I have read that the diode bridge will bring the voltage up.
   
  However, the transformer is currently hooked up to a power supply circuit.
  The voltage on the other side of the rectifier is ~35Volts. Actually lower.
  What do you make of that? Half wave rectifier?
   
  I agree with you on your other points.
  HRMM


----------



## tomb

Quote: 





nullstring said:


> This is where I am a bit confused. I have read that the diode bridge will bring the voltage up.
> 
> However, the transformer is currently hooked up to a power supply circuit.
> The voltage on the other side of the rectifier is ~35Volts. Actually lower.
> ...


 

 Cobaltmute was calculating the absolute worst case for the purposes of spec'ng the voltage of the filter capacitor, which is right and proper.
   
  However, there are a number of things that can affect that final rectified voltage.  For instance, is that 38VAC you reference a measured voltage and did you measure it with an RMS-capable DMM?  Only the better, more expensive DMM's can accurately measure VAC RMS voltage.  Cheaper meters may be measuring Vp, which will be much higher.  If the voltage is spec'd at 38VAC by the mfr, is that spec'd at 120V mains?  If so, mains in the US may easily vary from 120 down to 110V.  That's almost a 10% drop, which could knock 3.8 volts off of that 38VAC, or 34.2VAC.
   
  The theoretical equation for rectifying VACrms is SQRT(2) * VACrms.  However, that doesn't account for the losses in the bridge rectifier, about 1.4V.  So, worst case (best case for the filter capacitor), you might have (1.414 * 34.2) - 1.4 = 46.9V.  This still results in a combination of AC ripple plus DC, represented by some remaining "valleys" between the crests of the voltage wave.  A typical correction factor of about 0.8-0.9 is applied for the smoothing factor provided by the capacitor.  This results in about 37.5VDC.  In truth, your DMM may only be able to measure the DC component of the recitfied voltage prior to the cap, which is probably that 37.5VDC.
   
  That's awfully close to your 35VDC - any dip in the transformer due to loading could be enough to bring it down to the 35VDC you've measured.  We need to know a bit more about your transformer and the setup you have to fully explain it, though.  Having had a lot of experience with 24VAC power supplies, I can tell you that a good rule of thumb is about 5 extra volts available prior to a regulator (~29V), using full-wave rectification, lots of filter capacitance, and a sizably-overrated current capacity on the 24VAC.  Even so, the filter cap voltage ratings spec'd under that scenario are 50V, not 35V.


----------



## cobaltmute

Well there is the note that you said "unloaded",
   
  Some transformers can have a significantly higher unloaded voltage.
   
  Do you know what the transformer is actually rated for?
   
  Inherently, by putting the regulator on the transformer you load it.


----------



## nullstring

Quote: 





tomb said:


> For instance, is that 38VAC you reference a measured voltage and did you measure it with an RMS-capable DMM?  Only the better, more expensive DMM's can accurately measure VAC RMS voltage.  Cheaper meters may be measuring Vp-p, which will be much higher.


 

 This is likely the issue.
  I have no idea what it's factory rated for.
  And I didn't realize that a transformer loaded by an unloaded regulator was still considered loaded.
   
  Thanks for the help guys. I really appreciate it.
  I will do more research, and likely create a separate thread.
   
  The only question that remains is.. what on earth is the transformer really..
   
   

 Measured 38 or 39"VAC" using cheap DMM while loaded by unloaded powersupply
 Power supply is a vintage satellite receiver power supply. Says 36V 4amps (at 6 minutes or something)
 Directly after the diode bridge, I measured 34or35VDC. I don't recall there being any capacitors at this point of the circuit, which seems very important. I'll have to recheck look tonight.
 After some research I've realized: If tomb is right about that reading being Vp-p Vp, then that number is actually the worst (or best) case V after the rectifier. 38-1.4 + ripple stuff =~ 34
 Solved =) 38/sqrt(2) = ~27VAC. That is likely the real transformer output.
   
  Thanks again =)
   
  EDIT: wait, what is Vp-p?
  I think it makes more sense that the DMM would be reporting the peak Voltage in one direction. Or Vp-p/2? Or Vp
  Vp-p would be WAY too high, and there is just no use reporting that.


----------



## tomb

You're correct - I shouldn't have said Vp-p, but just Vp.


----------



## nullstring

Well, turns out I was wrong.
   

 I have no idea what the transformer is rated for.
 Measured 38 or 39"VAC" using cheap DMM while loaded by unloaded powersupply. *relooked, as far as I can tell, the only thing in the circuit is a diode bridge and a two relays. *Perhaps it is unloaded after all.
 Power supply is a vintage satellite receiver power supply. Says 36V 4amps (at 6 minutes or something)
 Directly after the diode bridge, I measured 34or35VDC. I don't recall there being any capacitors at this point of the circuit, which seems very important. I'll have to recheck look tonight.
 After some research I've realized: If tomb is right about that reading being Vp-p Vp, then that number is actually the worst (or best) case V after the rectifier. 38-1.4 + ripple stuff =~ 34 This is all wrong because of the point below.
 *Measured 120VAC off of a wall socket.*
 I rechecked, and there aren't any capacitors after the diode bridge. My new hypothesis is that multimeter has no idea how to measure that, because it should look like a absolute value'd sin wave. I should add to a cap to the circuit to see if that changes things....


----------



## cobaltmute

Just as an update, prototype boards are on their way from tomb to myself.  Once I've done tests to ensure that the BOM creates functional boards, they will be made available.


----------



## TheShaman

Good to know. Keep up the good work guys!


----------



## cobaltmute

I received prototype boards yesterday and in a fit of "I can do that other stuff later" built a 5V output one.
   
  I would say that the build is straight-forward and easy to complete.  I didn't get the sense while assembling the regulator that it was a tight build, but when you finish and look at it you realize there is a fair amount of parts in a small space.  You definitely want to take your time to ensure that you get the parts down in the right place the first time, as it is challenging to change parts on the board afterwards. 
   
  And change parts I did.  There is always a slight issue when you use one part footprint (FET) for another (depletion-mode MOSFET). That means that for the prototype boards Q2, the LND150, needs to be installed turned around 180 degrees compared to the footprint on the board.
   
  As for performance, all I got to do last nite was having a working reg that output 4.99V as shown on my meter as I needed to go to sleep.  I did see that the start-up behavior was that, for the 5V version, it quickly started to ~4V and then over about 5 seconds the voltage came up and stabilized at the 4.99V final output voltage.  This is expected as the low pass filter on the reference voltage charges.
   
  So what now?  Well, I want to personally build two more regulators, one each with the other reference options, to ensure that any prototyper gets a functional board when they build from the BOM.  I may get one done this week, but I'm not sure about having both done.  After I get the two built, I figure they'll be ready for the rest of you.


----------



## MASantos

This looks like a nice little regulator! It's small enough to be built inside a large wallwart with a trafo for small power applications, should be perfect for a Y2 or small desktop amp.

Should be looking for a few of these boards when available. 

A kit from beezar or glassjaraudio would be a great thing!!


----------



## cobaltmute

Some pics of the built unit:
   

   

   
  And yes, before someone says something, the 1000uF filter cap is not a Panasonic.  Turns out that when I went to build, it seems that I forgot to order that part, so I pulled something out of my parts box.  And these pictures were taken before I turned Q2 around.


----------



## c12mech

You were not kidding about it looking tight on the board. 
   
  Was max voltage and current discussed for this.  I thought I read it somewhere but can't seem to find it now.  It seems a couple of these could be used to make a nice multiple voltage bench power supply.


----------



## rds

awesome!


----------



## elliot42

That looks great. It's so tiny!


----------



## Beftus

All I cab say is: wow! And: when and where can I buy a kit?


----------



## cobaltmute

Thanks for the compliments.  Tangent should get the original kudos for the size of the TREAD - I just tried to shove a bunch of parts in the same size  
	

	
	
		
		

		
			




   
  Choosing some boards that a whole bunch of people have built as reference, the grubDAC/SkeletonDAC/BantamDAC are ~51x27mm rounding up.  The r1 is 53mmx33mm or for the less metrically inclined ~2"x1.25".  So yes it is tiny.  It is not the tiniest thing I've built, but for some reason everything I design is small.


----------



## Avro_Arrow

I would turn the heat sink around so it is away from the capacitor unless
  space is an issue.


----------



## cobaltmute

Quote: 





c12mech said:


> Was max voltage and current discussed for this.  I thought I read it somewhere but can't seem to find it now.  It seems a couple of these could be used to make a nice multiple voltage bench power supply.


 

 I may have answered this, but I'm going to again, as I can't bother be bothered looking back through the thread.
   
  First to answer this in terms of the schematic and the PCB.  Looking at it generically, the limiting factors on the regulator are:

 The dissipation in R3, but this can be jumpered so it really is not an issue
 The voltage rating of C3 versus the capacitance rating to provide a good ripple filter.
 The value of R4 which acts as a current limit to the base of the pass transistor
 The dissipation (and therefore heatsinking) of Q1, the pass transistor
 The voltage rating of the other parts (like the op-amp and the capacitors0
 The current capacity of the traces - if you are really trying to push the boundaries.
   
  The critical factors that I see are the dissipation of Q1 and the ratings on C3.  Q1 can be heatsinked off board, so that is not so much of an issue as C3.  Higher current draw requires higher capacitance which also requires a larger footprint for a given voltage rating.  "A given voltage rating" is critical - if you feed the board AC, you want a good safety margin, but if you were to feed the board DC, you can get away with a lot higher input voltage with the same parts.  With a very quick check at Digikey, I'd say if you want to stay within the footprints of the board, 33-34V is about the maximum output voltage of the PCB.
   
  Now to answer this in regards to the BOM that I have posted.  Capacitors on the output side are rated for 25V, so I set the maximum on the output to be 24V.  I've also set R4 so that the approximate maximum output current is 250ma. This limit was set completely arbitrarily, so you could push up the current output limit as required.  While some may say having a current limit in the supply is a bad thing, if you've ever had your supply go into limit due to a build mistake, you can appreciate its value.


----------



## cobaltmute

Quote: 





avro_arrow said:


> I would turn the heat sink around so it is away from the capacitor unless
> space is an issue.


 

 No issue.  It was only put over the board to prove that it would fit.


----------



## francisdemarte

Great work!


----------



## tomb

Quote: 





francisdemarte said:


> Great work!


 

 Agreed!  Very impressive!


----------



## rds

Quote: 





cobaltmute said:


> No issue.  It was only put over the board to prove that it would fit.


 


  Although it technically fits it's probably not a reasonable build option since there is a good chance of direct thermal contact to the capacitors on either side.   This could be rectified in the production version by moving R3 down, turning it 90 degrees clockwise and moving C3 as close to the board edge as possible.  This should gain you at least 3mm that can be used to provide reasonable space on either side of the heat sink.


----------



## Billyk

Nice!! It will be a perfect fit for many of my projects!!!


----------



## cobaltmute

Quote: 





rds said:


> Although it technically fits it's probably not a reasonable build option since there is a good chance of direct thermal contact to the capacitors on either side.   This could be rectified in the production version by moving R3 down, turning it 90 degrees clockwise and moving C3 as close to the board edge as possible.  This should gain you at least 3mm that can be used to provide reasonable space on either side of the heat sink.


 
   
  I may agree about the heatsink over the board.  Looking at my build there is ~1mm of clearance on either side of the heatsink to the caps.  These Mouser parts may be OK for off board 532-581202B25G, 567-634-10ABP
   
  However, moving C3 around is not as feasible as you make it out to be.  The cap in the picture is 16mm, but if you use the heatsink  facing off-board, there is room for an 18mm cap.  Most I can move over an 18mm cap is 1.5mm (to maintain clearance around the mounting hole and diode bridge) - and that kills R3 totally.


----------



## rds

cobaltmute said:


> However, moving C3 around is not as feasible as you make it out to be.  The cap in the picture is 16mm, but if you use the heatsink  facing off-board, there is room for an 18mm cap.  Most I can move over an 18mm cap is 1.5mm (to maintain clearance around the mounting hole and diode bridge) - and that kills R3 totally.




So I guess it's a design choice between having an 18mm cap option and having the option of mounting the heat sink inside the board. To me the latter is more useful and is necessary if you want to claim that the regulator only occupies the space of the board.


----------



## cobaltmute

Quote:


rds said:


> So I guess it's a design choice between having an 18mm cap option and having the option of mounting the heat sink inside the board. To me the latter is more useful and is necessary if you want to claim that the regulator only occupies the space of the board.


 
   
  You have a point. Let me play a bit when I'm not at work.


----------



## tangent

It's easy to bend the fins on the heat sink with needle nose pliers, curling them inward to make room for the bigger cap.


----------



## tomb

A limited number of prototype PCB's are now available.
   
  Also, please reference the r1 proto webpage:
r1 prototype
  You'll find the BOM and other pertinent data.


----------



## cobaltmute

tomb did forget this link:
   
http://beezar.com/catalog/product_info.php?cPath=25&products_id=137
   
  As one can ascertain,  I asked tomb to handle the distribution of the prototype boards that I ordered.  He has all the stuff to handle shipping PCBs and I don't.  Also as many are in the US it provides much faster shipping than from me.
   
  By tomb putting these up, it also implies that within the limits of the testing that I can do, the boards/BOM is functional.  The only thing that needs to be done is to install Q2 rotated 180 degrees.
   
  As rds noted earlier in the thread, he was willing to test a regulator.  There is a 5V version of the regulator on its way to him and he is going to try to do some testing when he can find some time in his busy schedule.  I personally don't have a LNMP for testing, but at least AC ripple was below what my Fluke could read.
   
  So enjoy and build.


----------



## tangent

Quote: 





cobaltmute said:


> tomb did forget this link:
> 
> http://beezar.com/catalog/product_info.php?cPath=25&products_id=137


 
   
  Um....I don't remember inventing any regulator technology. I wrote up some history and made an implementation of a different circuit than used for the r1. That's all.


----------



## cobaltmute

Now that I'm awake and having read the Beezar r1 page in detail (which I hadn't last nite), I will agree that the line that you are pointing out is mis-worded.  It would seem that tomb was attempting to give you credit for the work that you have done and it didn't come out quite right.
   
  I have sent tomb what my preferred wording would be and have asked him to update the store page


----------



## tangent

The record here in this thread is sufficient. I helped with the layout, and that's all here.


----------



## cobaltmute

The sentence in question has been updated.


----------



## Billyk

Ordered my boards! Thanks to all much appreciated!!!


----------



## Billyk

Hey now.I am having a bit of trouble sourcing the op-amp LT1677. Any Ideas?Thanks


----------



## nullstring

http://search.digikey.com/scripts/DkSearch/dksus.dll?Detail&name=LT1677CS8%23PBF-ND


----------



## cobaltmute

Digikey has ~2700 in-stock of the LT1677.  Preferred part number LT1677CS8#PBF-ND
   
   
  EDIT:  And as a note, I chose parts that require orders from both Digikey and Mouser.  There may be alternatives, but I chose what I believe to be the best part for each position ( though of course I can always be convinced otherwise)


----------



## Billyk

Thanks!
   I am embarrassed, I swear they said 0 stock when I checked this afternoon. It's a good thing I didn't place my order yet!


----------



## cobaltmute

This has been strangely quiet from you all.
   
  I know boards have been shipped to people.  Has anyone, beside me, built one? If so, any feedback?
   
  Usually by this point there would have been some questions.


----------



## cobaltmute

Someone asked recently about using the r1 as a heater supply for 6.3V, 600ma - I would say it is definitely doable.
   
  Bom parts would be as follows:
  R3 - jumper
 R6 - 649 Ohms (6.35V output) or 661 Ohms (6.26V output)
 D1 -1N5230B
 U2 - LM336BZ-2.5
 R7 - CMF55274R00FHEB
 C3 - EEU-FC1E562
 R4 - 80 Ohms - CMF5578R700FHEB
 Q1 needs to be mounted on a good heatsink.
 Transformer - 9VAC output
   
  Given the hfe of Q1, per datasheet minimum this config will deliver 900ma, but using the typical hfe graph on the OnSemi datasheet, it will be more like 1.5A.


----------



## Blooze

That'd be me Erik!!!  I'm looking at using it for a preamp that already has a LM317 implementation in it's schematic for the heaters (2 x 300mA), but I figure for a few more $$$ I can have super quiet DC on the heaters which would work great for a pre and something that looks better than a cobbled up perfboard.  I can think of several other projects where this would work well for the same job.
   
  Thanks for figuring out the parts requirements for me.  The transformer has an 8V/1.5A secondary winding that I figure will run more like 9V anyway with my high mains voltage, so those numbers should be good.  Any recommendations for a heatsink?
   
  Just checking.............Would R6 be 649 ohms or 3.8K?  If I use the calculator on the BOM sheet using a reference voltage of 5V and R5=1000, then 3.8K gives me 6.3V out.  649 ohms gives me 12.7V out.


----------



## cobaltmute

Well, the issue with R6, is that I would recommend the 2.5V reference, as I listed in the post above rather than the 5V reference.  The reason is that you'll get better start up performance out of the bootstrap on the regulator.  Using the 5V reference for 6.3V can be done, but the component choice for D1 becomes critical to ensure proper start up and I haven't had enough sleep lately to find a good part.
   
  So R6 would be 649 Ohms for the 2.5V reference.  If you wanted to use 5V reference (LM336BZ-5 for U2), you can use the the 3.83K, but use something like a 5.7-5.9V zener for D1.
   
  As for a heatsink, you'll be getting ~12V after the bridge.  5.7V drop in Q1 @ 600ma = ~3.4W of heat to be dissipated.  I might try something like this with the fins oriented off the board:
http://ca.mouser.com/ProductDetail/Aavid-Thermalloy/7023B-MTG/?qs=sGAEpiMZZMttgyDkZ5WiusUw%252bQXhbmeCbGT4Q7lNLYE%3d


----------



## Blooze

Duh.  Didn't see the 2.5 on U2.  Now it makes sense.  Thanks for all your help.  Plan on ordering later this week after the paycheck with expendable income arrives.  Gotta stick to the budget and all.


----------



## cobaltmute

Quote: 





cobaltmute said:


> Someone asked recently about using the r1 as a heater supply for 6.3V, 600ma - I would say it is definitely doable.
> 
> Bom parts would be as follows:
> R3 - jumper
> ...


 

 Ok, a note about R3.  A jumper is easy and you don't have to worry about dissipation.
   
  That being said, you could put a power resistor in for R3, say something like this: http://ca.mouser.com/ProductDetail/Bourns/PWR221T-30-4R70J/?qs=sGAEpiMZZMsPqMdJzcrNwqJAQmshBUYlGg%252b3d6X9QRo%3d
   
  You dissipate about 1.8W in that resistor, but you get some other benefits.  A really nice one is that R3/C3 would form a low pass filter with a corner of 6Hz, helping reduce noise.  That resistor is rated for 2.25W in free air, so you could likely use a small heatsink like this: http://ca.mouser.com/ProductDetail/Aavid-Thermalloy/577202B00000G/?qs=sGAEpiMZZMttgyDkZ5Wiut26jWwHqNF9cgDmGgnRNkQ%3d or the same one I suggested for Q1.
   
  Edit:  And as a side effect, you split the heat dissipated total to both R3 and Q1.


----------



## glt

Very nice project.
  What is the voltage headroom required to keep Q1 going? (the voltage headroom after R3)
  Also what are the simulations results?
   
  Thanks


----------



## tomb

OK guys - what gives?  I've sold all 29 prototypes that were available and no one who bought one has posted a dang thing.  Haven't any of you built one, yet?


----------



## Blooze

Quote: 





tomb said:


> OK guys - what gives?  I've sold all 29 prototypes that were available and no one who bought one has posted a dang thing.  Haven't any of you built one, yet?


 


  Sorry about that Tom.  My amp and preamp projects got put on hold for a bit so I haven't populated the boards, but I see no reason why they wouldn't work very well for filament regulators, especially in my preamp project where quiet is better.  My preamp is awaiting the implementation of a friends remote control design into the existing schematic, but I'm hoping it will be ready to start in a month or so.


----------



## tomb

Quote: 





blooze said:


> Sorry about that Tom.  My amp and preamp projects got put on hold for a bit so I haven't populated the boards, but I see no reason why they wouldn't work very well for filament regulators, especially in my preamp project where quiet is better.  My preamp is awaiting the implementation of a friends remote control design into the existing schematic, but I'm hoping it will be ready to start in a month or so.


 

 Well at least you posted, Blooze - even if you haven't built one, yet.  Thanks!!
   
  I'm going to build one next weekend and let you all know how it turns out.


----------



## cobaltmute

Quote: 





tomb said:


> OK guys - what gives?  I've sold all 29 prototypes that were available and no one who bought one has posted a dang thing.  Haven't any of you built one, yet?


 
   
  Maybe it is such a stunning design with such awesome docs and ease to build that no-one has to ever ask any question about it.  Ever.
   
  And if you believe that I've got a small tropical island to sell you at a great price.


----------



## tcpoint

Just started a board late last night.  Will probably finish either Tuesday or Wednesday (Got to take the kids trick or treatin' tonight).  Will let you know how it goes.  I expect it will just work.
   
  I plan on making one 9V PS and a +/-15V (with the other two board).


----------



## tomb

Sounds great!  I'm delayed, as usual - hope to get to it this weekend.


----------



## tcpoint

Put together a 9 V board and it works great.  Thanks for putting together this project.


----------



## tomb

Quote: 





tcpoint said:


> Put together a 9 V board and it works great.  Thanks for putting together this project.


 

 Excellent!


----------



## cobaltmute

Quote: 





tcpoint said:


> Put together a 9 V board and it works great.  Thanks for putting together this project.


 

 Any comments about the build process?  Or pictures?


----------



## tcpoint

The build was pretty straight forward.  It just worked first try.  I was pretty careful and took my time. The parts all fit easily.  The only things I'd change are Q2 and add a silk screen on the bottom (which I'm sure you already have your your list for the production boards).  I'll post pictures when I finish my +/- 15V boards.  They will be more interesting.


----------



## tomb

I finally got one of these built myself -
   






   
  My LNMP is out of commission temporarily, but I'll have some measurements when it's available.  I haven't plugged it in yet, but will try to later today or tomorrow.  I built it for 24VDC and everything should be OK - Q2 is reversed and that was the main thing.
	

	
	
		
		

		
			




   
  EDIT:  Looks like I didn't edit the second photo link after copying and pasting it.  It should show two separate pics, now.


----------



## noveltone

Looks like a really great, compact build. Thanks for sharing your builds, guys. I'm curious to see what LNMP says. I've started up the LNMP project myself. Any word on production for these boards? I have some old TREAD boards but I'd like to try this for a turntable project.


----------



## tomb

Quote: 





noveltone said:


> Looks like a really great, compact build. Thanks for sharing your builds, guys. I'm curious to see what LNMP says. I've started up the LNMP project myself. Any word on production for these boards? I have some old TREAD boards but I'd like to try this for a turntable project.


 

 Cobaltmute and I agree that we want documented measurements before ordering a production run.  Hopefully, mine will be repaired soon and I'll have some hard data to report.


----------



## Yoga Flame

I finally was able to set aside time to assemble my prototype. Better late than never I suppose. Did not run into any real difficulties. The location of pin 1 on the opamp was not obvious to me, but the posted photos helped. Had to look up the schematic to confirm which pads C2 was supposed to be placed on, which is arguably a good thing. Thanks cobaltmute, tomb, and everyone!


----------



## tomb

Looks great!


----------



## mfuerst

Quote: 





tomb said:


> OK guys - what gives?  I've sold all 29 prototypes that were available and no one who bought one has posted a dang thing.  Haven't any of you built one, yet?


 


 Hi tomb,
   
  I hope these pics will make you happy:
   

   

   

   

   
   
  Also follow this link to see the finished product:
http://www.head-fi.org/t/419563/the-pimeta-v2-thread/420#post_8289096
   
  Thanks for designing this - really reliable and very stable so far.
   
  Cheers!


----------



## tomb

Very nice!  I know cobaltmute is still hoping someone will test his design.  Has anyone put a scope to one, yet?  I'm still waiting on my LNMP to get fixed.


----------



## rds

I am the jerk who's had cobaltmute's r1 for over a year and still have not tested it. I didn't realize how busy my life would be and entering a program at a new school where I don't do anything with electronics has made it difficult to get a hold of equipment. ..okay these are poor excuses.
   
  I have located the equipment I need and plan to make these measurements within a month (I imagine cobaltmute rolling his eyes right now). Really I'm pledging to get this done and am looking forward to the results.


----------



## cobaltmute

rds, 

Plain and simple "Life happens".

With the number of people that are waiting for me to finish what I'm doing with the pupDAC, I can't be one to point fingers. I'm just as guilty as you are.


----------



## walangalam

any updates?


----------



## tomb

Dsavitsk has fixed my LNMP!  I have it in hand and will test the R1 under a Millett Hybrid load this weekend.  I'll let you all know.


----------



## tcpoint

Quote: 





tomb said:


> Dsavitsk has fixed my LNMP!  I have it in hand and will test the R1 under a Millett Hybrid load this weekend.  I'll let you all know.


 

 That is great news.


----------



## Mullet

When available to the general public, is it possible to use two of these to create a bi-polar power supply?


----------



## cobaltmute

This could be run as a dual supply in the same way the TREAD could be run as one:

http://web.archive.org/web/20100822022109/http://tangentsoft.net/elec/tread/pguide.html#dual


----------



## tomb

Looks like I blew the build, guys. 
	

	
	
		
		

		
			





   I got R6 and R7 correct, but I neglected to order the correct versions for D1 and U2 at 24V output.  I can't get any more than ~8.6VDC on the output and I don't have a load that low to test.
   
  I'll have the right parts on order today.


----------



## Mullet

What ever happened to this project?


----------



## tomb

Quote: 





mullet said:


> What ever happened to this project?


 
  Umm ... unfortunately, it's in my lap.  I built one for the purpose of making specific measurements using Tangent's LNMP.  However, my LNMP batteries shorted out, made a mess and blew up the TLE chip.  Dsavitsk fixed it for me, since I was pretty busy at the time, but then I blew out the r1 I built.  (I put too much voltage and current load on it.)  I have all the parts to build a new one, but just haven't got 'round to it, yet.


----------



## KimLaroux

Quote: 





tomb said:


> Umm ... unfortunately, it's in my lap.  I built one for the purpose of making specific measurements using Tangent's LNMP.  However, my LNMP batteries shorted out, made a mess and blew up the TLE chip.  Dsavitsk fixed it for me, since I was pretty busy at the time, but then I blew out the r1 I built. * (I put too much voltage and current load on it.)*  I have all the parts to build a new one, but just haven't got 'round to it, yet.


 
   
  Does this mean you now know what maximum voltage and current it can feed? I'd be interested in those numbers.


----------



## tomb

Quote: 





kimlaroux said:


> Does this mean you now know what maximum voltage and current it can feed? I'd be interested in those numbers.


 
  Just going from memory, but I think cobaltmute indicated that there's no problem exceeding what I did - it's just that the parts selection at present was not set up for that much.


----------



## Mullet

I have a few projects that would benefit from a board like this. I'm thinking of going with a Salas v1.1 BiB which might be overkill. Or a Sigma 25, which might be in the same league. I like that the size is super small and flexible.


----------



## walangalam

yeah me too.  I have a dynalo I need to  recase and it just needs a reg like this


----------



## cobaltmute

kimlaroux said:


> Does this mean you now know what maximum voltage and current it can feed? I'd be interested in those numbers.




I'll admit to not having looked at the circuit in quite a while so it would take me a few moments to figure out the limits with the "default" BOM we spec'ed. That doesn't mean that you can't spec out a different set of parts to meet a specific need. With the proper choices for parts (and heat-sinking), the practical limit will be the copper traces on the board.


----------



## amcananey

What a fascinating thread. I just read through the whole thing. I probably understood 2% of it, but it was great to see how the project developed. It's too bad it's been languishing a bit, however...
   
  Question: would it be feasible to build several of these to use as bench power supplies? Maybe a 3V, a 5V, a 6V and a 12V? Other than continually adjustable voltage, what would the benefit of a bench power supply be?
   
  Best regards,
 Adam


----------



## amcananey

Is this project officially dead? I'm looking for a small, low-cost 6.3V power supply and I thought this might be perfect, but...


----------



## tomb

Quote: 





amcananey said:


> Is this project officially dead? I'm looking for a small, low-cost 6.3V power supply and I thought this might be perfect, but...


 
  No, it's not dead - just in suspended animation because of me.  I'll try to do better.


----------



## amcananey

Not trying to pressure anyone - you don't owe me anything and if this ever comes to fruition, I'll be grateful for the work you and everyone else has done. Thanks for the update -- glad to hear it isn't dead!


----------



## Forte

Any progress?


----------



## individual6891

Sorry for the thread revival. Any updates after all this time?


----------



## tomb

individual6891 said:


> Sorry for the thread revival. Any updates after all this time?


We had another builder who built one a few years ago, but couldn't get it to stabilize.  I never took the chance to go back to it after that, unfortunately.


----------



## individual6891

tomb said:


> We had another builder who built one a few years ago, but couldn't get it to stabilize.  I never took the chance to go back to it after that, unfortunately.


Ahhh, no worries. Thanks for looking at it. When you say stabilise, do you mean oscillation? or a different factor?


----------



## tomb

individual6891 said:


> Ahhh, no worries. Thanks for looking at it. When you say stabilise, do you mean oscillation? or a different factor?


Oscillation.


----------



## Billyk

I have a couple of Ver. .28 boards. Would it be worthwhile trying to build one?


----------



## Blooze

Mine oscillated as well. Tomb, it’s surprising no one has just put out another board like the Tread. I’d use them fairly often. Small, tidy, and worked well. I know there are some others out there, but they’re slightly larger and cost more to build.


----------



## tomb

Blooze said:


> Mine oscillated as well. Tomb, it’s surprising no one has just put out another board like the Tread. I’d use them fairly often. Small, tidy, and worked well. I know there are some others out there, but they’re slightly larger and cost more to build.


Agreed.

Maybe we'll do something about that.


----------



## Blooze

tomb said:


> Agreed.
> 
> Maybe we'll do something about that.



If I could focus long enough to learn Kicad or Diptrace I’d just lay one out exactly like the Tread and make my own. I can lay one out on perfboard, but it’s a hassle.


----------



## Billyk

Thanks!
Tread was nice little board. There's always Ti's Sigma 25 and 26.
Just came across the boards, I bought them just before I got sick.


----------



## Blooze

Billyk said:


> Thanks!
> Tread was nice little board. There's always Ti's Sigma 25 and 26.
> Just came across the boards, I bought them just before I got sick.


Yep. Twisted Pear has a few as well. The nice thing about the TREAD was you could get the board and build it for less than just the boards from the alternatives.


----------

