My PCB design of Salas SHunt Reg

Lazybutt · 3rd July 2011, 05:30 AM

Hello all,

Here is my version of the Salas Shunt Reg SSLV1.1 which I show here courtesy of Salas.
This is based on the same schematic as the one from the BiB group Buy proposed on this forum.

The spirit of this PCB is:
- As compact as possible
- Flexible Positive / negative by jumper configuration
- 1 x 22mm or 2 x 18mm electrolytics at the input + MKP bypass
- Possibility to use electrolytics to big MKP caps (I have some big 4.7uF Wima MKP10 that I want to use..) at the output
- Possibility of bypassing of sensing wires by jumper or resistor

I am looking for experts opinion, criticism and advices on the PCB layout. From general comments on the components placement, grounding, tracks routing, use of the 2 layers, etc.... basically anything that could help me make it a better design.
One thing I'm most interested in is comments on the grounding.. would I benefit from a ground plane as opposed to star grounding as it is now ? or Could I combine both ? etc..?

This is my first attempt at designing a PCB, and I know there are some (intentional) trade offs, but I am not sure of there significance so I really won't feel offended by any comment. It's open bar ...

Thanks a lot !

PS: Most useful comment by mid-July gets a free pair of PCB Postage paid (ok subjectively and unilaterally judged by me :P)

Piersma · 3rd July 2011, 01:27 PM

For convinience, please post also the the schematic.
The heatsinks are too close to the edge.

Lazybutt · 3rd July 2011, 04:28 PM

Here is the schematic

The heatsinks are actually ON the edge... this is intentional as I believe I will use the chassis as a heatsink.... if not, I put them here just to make sure there is enough space around them and other components. I did not see the matter with the heatsinks not having PCB underneath them . But maybe I miss something ?

AndrewT · 3rd July 2011, 06:21 PM

for Q3, use 2sk117gr, or better use 2sk170bl

hesener · 4th July 2011, 08:32 AM

Hi,

just some comments:
- bottom side: the connection from C5 to R1 and D2 is strange, it should be a straight connection and not go over to be so close to C1. There is very little inductive compensation you will achieve at such short runs, and the PCB inbetween
- bottom side: the GND wire that passes above C2 (upper righthand corner) is very close to that pad of C2, personally I would make that spacing wider or have the trace on top
- all traces where current is flowing should be as "rectangular" as possible, copper comes for free so just use it to widen the traces and add rectangles where they fit
- what is the purpose of having C3 and C4 sit inside each other, will one of them be stuffed from the bottom?
- agree with Piersma on the location of the heatsinks, they exist with solderable pins giving a very good mechanical connection to the PCB, so you may want to look into that.
- output GND is connected to the input caps only with one VIA at star ground, so your output current will have to pass through a smallish amount of tin inside a little hole... not ideal.. at least you may want to solder a piece of wire into this hole, to fill it with metal.
- the wires around your star ground seem all very thin. As the ground plane is on the top layer anyway, my recommendation would be to have a lot more copper on these connections.
- personally, I would do the reverse however, put a large ground plane with all the right connections on the bottom layer, and have all signal wires on the top layer, which - combined with labels - makes for much easier measuring and debugging. With designing a star ground on the PCB, you are forcing the location without real need to put it there (and not much noise improvement either), but reducing the available amount of copper to carry the current. Better to have a proper star ground at the input of your amplifier.
- no test points on your PCB. I guess that wanting to have a compact PCB leaves not much space for these (and your design is quite compact!), but they do come in handy especially for the first run

just my two cents...

Guido Tent · 4th July 2011, 08:44 AM

Quote:

Originally Posted by Lazybutt

Hello all,

I am looking for experts opinion, criticism and advices on the PCB layout. [/B]

I have written a short article which covers most important layout aspects, see

http://www.tentlabs.com/InfoSupport/...decoupling.pdf

best

AndrewT · 08:58 AM

I remember reading that about a decade ago. Thank you.
I still have the copy in my electronic reference files.

Maybe more importantly I have re-read it twice over the years. As I learn more, I get more from it.

hesener · 4th July 2011, 12:26 PM

Very nice document with excellent insight, thanks

Lazybutt · 4th July 2011, 03:31 PM

Quote: