A TREAD sized regulator - the r1
Mar 8, 2011 at 10:23 AM Post #46 of 189
In the first link, it certainly goes to the input cap 
confused.gif

 
You have a starground with C1 (input cap), R20 (Q2 for you), the opamp ground, going to a terminal labelled "unreg. gnd"
 
Mar 8, 2011 at 10:33 AM Post #47 of 189


Quote:
In the first link, it certainly goes to the input cap 
confused.gif

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

 
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.
 
Mar 8, 2011 at 11:17 AM Post #48 of 189
 
Quote:
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 
wink.gif

 
Mar 8, 2011 at 11:23 AM Post #49 of 189


Quote:
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.
 
 
Mar 8, 2011 at 2:40 PM Post #50 of 189


Quote:
...
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.
 
Mar 8, 2011 at 3:13 PM Post #51 of 189
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.
 
Mar 8, 2011 at 3:28 PM Post #52 of 189


Quote:
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 :wink:  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 
evil_smiley.gif

 
Mar 11, 2011 at 10:46 AM Post #53 of 189
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:

 
 
Mar 11, 2011 at 11:46 AM Post #54 of 189
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.
 
 
Mar 11, 2011 at 12:58 PM Post #55 of 189
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.
 
 
 
Mar 11, 2011 at 1:25 PM Post #56 of 189


Quote:
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
 
 
Mar 11, 2011 at 3:42 PM Post #58 of 189


Quote:
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.
 
 
 
Mar 11, 2011 at 7:56 PM Post #59 of 189
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.
 
Mar 12, 2011 at 2:04 AM Post #60 of 189


Quote:
@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.
 
 

Users who are viewing this thread

Back
Top