My PCB design of Salas SHunt Reg - diyAudio
Go Back   Home > Forums > Amplifiers > Power Supplies

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 3rd July 2011, 05:30 AM   #1
diyAudio Member
 
Join Date: Mar 2009
Default My PCB design of Salas SHunt Reg

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

Click the image to open in full size.

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)
  Reply With Quote
Old 3rd July 2011, 01:27 PM   #2
Piersma is offline Piersma  Netherlands
diyAudio Member
 
Piersma's Avatar
 
Join Date: Jan 2003
Location: Netherlands
Default Schematic

For convinience, please post also the the schematic.
The heatsinks are too close to the edge.
  Reply With Quote
Old 3rd July 2011, 04:28 PM   #3
diyAudio Member
 
Join Date: Mar 2009
Here is the schematic

Click the image to open in full size.


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 ?
  Reply With Quote
Old 3rd July 2011, 06:21 PM   #4
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
for Q3, use 2sk117gr, or better use 2sk170bl
__________________
regards Andrew T.
  Reply With Quote
Old 4th July 2011, 08:32 AM   #5
hesener is offline hesener  Germany
diyAudio Member
 
Join Date: Mar 2005
Location: Munich, Germany
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...
  Reply With Quote
Old 4th July 2011, 08:44 AM   #6
diyAudio Member
 
Join Date: Dec 2001
Location: Eindhoven
Quote:
Originally Posted by Lazybutt View Post
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
__________________
Guido Tent
www.Tentlabs.com
  Reply With Quote
Old 4th July 2011, 08:55 AM   #7
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
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.
__________________
regards Andrew T.

Last edited by AndrewT; 4th July 2011 at 08:58 AM.
  Reply With Quote
Old 4th July 2011, 12:26 PM   #8
hesener is offline hesener  Germany
diyAudio Member
 
Join Date: Mar 2005
Location: Munich, Germany
Very nice document with excellent insight, thanks
  Reply With Quote
Old 4th July 2011, 03:31 PM   #9
diyAudio Member
 
Join Date: Mar 2009
Quote:
Originally Posted by hesener View Post
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
The reason is I wanted to use C5a as the ground star. and wanted to avoid creating a ground loop by going back to C5d or C5b ground. There are heavy currents flowing in the first capacitors. Not sure I understood correctly, but the technique seems to be described in Guido's paper on layout


Quote:
Originally Posted by hesener View Post
- 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
2 good points, ... modifications under way !


Quote:
Originally Posted by hesener View Post
- what is the purpose of having C3 and C4 sit inside each other, will one of them be stuffed from the bottom?
That is to give the choice of either electrolytic OR MKT + resistor as specified by Salas in the manual. They're not intended to be used sinultaneously

Quote:
Originally Posted by hesener View Post
- 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.
Yes that one made me struggle for a while.... but I decided that way as it would also increase the lead length on the FETs if I decided to bolt them on the chassis


Quote:
Originally Posted by hesener View Post
- 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.
That's what I thought too.. until I realized it would be filled with the Capacitor lead and completely filled with solder anyway... but now I may want to make a few changes....

Quote:
Originally Posted by hesener View Post
- 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.
Hmmmm and yet I did my best to put as much copper there as I could... seems that's still not enough. You're right that my strategy of placing a C there forces me to do things in a certain way, possibly not ideal..

Quote:
Originally Posted by hesener View Post
- 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.
Very good idea ! I'll give it a thought!! although I have to disagree on the debuging part... once all components are there it's a nightmare to track back the path of signals since you cannot see the traces anymore...

Quote:
Originally Posted by hesener View Post
Better to have a proper star ground at the input of your amplifier.
I was planning to have a proper star ground at the input in addition to that one. Is there a problem with having little islands of stars connected together at the major star in the amp ?

Quote:
Originally Posted by hesener View Post
- no test points on your PCB
Absolutely! and I also wanted some... my problem is just that I did not yet figure out how to create them with Eagle :P

Quote:
Originally Posted by hesener View Post
just my two cents...
Hey , to me it's worth much more than 2 cents ! good food for thought, Thanks a lot !

Fred
  Reply With Quote
Old 4th July 2011, 03:35 PM   #10
diyAudio Member
 
Join Date: Mar 2009
Guido, Thanks a lot !
Very interesting indeed. Although I must admit, being a mechanical engineer I am lacking a lot of the background needed to understand the why's and how's ...

Also it makes me realize my search for the perfect PCB may be a little bit over engineering when I see the frequencies at play... hmmm 2.4Mhz .... all I'll be doing with that shunt reg will remain within audio frequency!
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
GB Thread for Salas SSLV1.1 BiB shunt reg Tea-Bag Group Buys 1471 1st September 2014 10:10 PM
FS : 2 x Salas low shunt Group-design by Salas korben69 Swap Meet 7 9th November 2011 10:06 PM
Wtd: Salas shunt reg boards RichLund Swap Meet 1 23rd April 2010 10:28 PM
Modified Salas Mosfet Shunt Reg mach1 Tubes / Valves 2 18th December 2008 05:36 AM


New To Site? Need Help?

All times are GMT. The time now is 08:45 AM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright 1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2