Head-Fi.org › Forums › Misc.-Category Forums › DIY (Do-It-Yourself) Discussions › A TREAD sized regulator - the r1
New Posts  All Forums:Forum Nav:

A TREAD sized regulator - the r1

post #1 of 178
Thread Starter 

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:

 

r1-0.7-schematic.png

 

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

r1-0.7-layout.png

 

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.

 

 

 


Edited by cobaltmute - 3/16/11 at 4:59pm
post #2 of 178

- 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  ;)

post #3 of 178

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?

post #4 of 178

Not CRC, RC  wink_face.gif

post #5 of 178
Thread Starter 
Quote:
Originally Posted by 00940 View Post

- 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  ;)


- 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.

 


Edited by cobaltmute - 3/2/11 at 9:28am
post #6 of 178
Thread Starter 
Quote:
Originally Posted by holland View Post

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.

 

post #7 of 178
Quote:
Originally Posted by 00940 View Post

Not CRC, RC  wink_face.gif



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.


Edited by holland - 3/2/11 at 9:56am
post #8 of 178

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 ?


Edited by 00940 - 3/2/11 at 9:34am
post #9 of 178
Quote:
Originally Posted by cobaltmute View Post




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.

post #10 of 178
Thread Starter 
Quote:
Originally Posted by 00940 View Post

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 ?


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.

 

 

 

post #11 of 178
Thread Starter 

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:

r1-r0.8-schematic.png

 

Board:

bcd6ca2f_r1-r0.8-all-layers.png

 

Thanks for the comments so far and keep them coming.


Edited by cobaltmute - 3/2/11 at 3:47pm
post #12 of 178

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.

post #13 of 178
Thread Starter 
Quote:
Originally Posted by 00940 View Post

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?

 

post #14 of 178

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

Here's roughly what I meant:

jung.gif


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.


Edited by 00940 - 3/3/11 at 5:59am
post #15 of 178
Thread Starter 

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...

New Posts  All Forums:Forum Nav:
  Return Home
Head-Fi.org › Forums › Misc.-Category Forums › DIY (Do-It-Yourself) Discussions › A TREAD sized regulator - the r1