My PCB design of Salas SHunt Reg

Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
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

Salas_eagle_V1.gif


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)
 
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 ?
 
Member
Joined 2005
Paid Member
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...
 
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


- 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 !


- 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

- 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


- 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....

- 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..

- 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...

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 ?

- 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

just my two cents...

Hey , to me it's worth much more than 2 cents ! good food for thought, Thanks a lot !

Fred
 
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!
 
Finally I decided to give up the idea to have a tiny tiny PCB, and made it a little bit bigger to accomodate most of your ideas... :)

It's still pretty small at 2.1"x3.3" and definitely is a clean design...(IMHO of course)!!
I also kept the idea of the star ground on the traces with high current, but combined to a ground plane for the best of both worlds!!

I spent a lot of time optimizing everything and here is the result:

Any new comments most welcome!
 

Attachments

  • Salas Shunt Top_V2.gif
    Salas Shunt Top_V2.gif
    65.3 KB · Views: 574
  • Salas Shunt Bottom_V2.gif
    Salas Shunt Bottom_V2.gif
    64 KB · Views: 559
I would personaly make the bottom layer one contigous ground, the splits wont do a lot in this instance, except create areas of copper that are only connected at one point:
http://www.hottconsultants.com/pdf_files/dipoles-1.pdf
http://w4trc.org/dipoles/dipoles-2.pdf
http://www.hottconsultants.com/pdf_files/dipoles-3.PDF
The father of EMC engineering:
http://www.hottconsultants.com/tips.html
Some good links at the back as well a a grounding in grounds:
http://www.x2y.com/filters/TechDay0...log_Designs_Demand_GoodPCBLayouts _JohnWu.pdf
 
Thanks Marce,

First off I want to say that I don't have a background in electronics, so my questions are really candid.

However, I don't understand how the Dipole papers apply to my ground plane.

Also on the paper from the father of EMC engineering (and most specifically the article on slots in the ground plane) I understand well that we should avoid creating ground loops, but it seems to me that what I'm doing is exactly the opposite. By connecting those areas of copper at only one point I believe I'm actually PREVENTING ground loops.

Maybe my MSPaint dirty drawing will explain better what I understood.

The reason for the splits is mainly to isolate the traces connecting the first 2 capacitors which carry heavy unfiltered current, which I want that to avoid being present on all the ground plane.

Again, no offense, I'm aware I may be wrong in my interpretation. I'll have a deeper look at those documents again anyway (my brain already dizzy)

Fred

Edit: Actually I have one ground loop on the plane, I'll correct it later
 

Attachments

  • Ground planes.gif
    Ground planes.gif
    5.1 KB · Views: 521
For most of the designs I do (exceptions being SMPS and Class D) I use a contigous solid ground plane with no slots, cuts etc. I would not worry about ground loops on simple designs like this, in fact I very rarely worry about ground loops on a PCB, as I use a solid ground and let the currents find there own path home.
The areas of copper that are only connected at one point will act as antennas, where we use ground copper pour on a design we always make shure there are at least two vias (preferably more) joining the copper pours to the main ground.
This link will give a brief intro into how currents flow on a PCB, and how important the return path is, dont think in terms of the electrons going round in a nice circle but how its illustrated in fig 2.
Printed Circuit Design & Fab Magazine Online
Rather a lot to get your head round, I know I've been doing PCB design and EMC for 25+ years and I am still studying nearly everyday as designs get more complex, clock speeds and rise times keep increasing, and the amount of RF pollution increases every year, causing more problems for keeping it out of equipement. That said, keep things simple, especialy grounds and your designs will work.
More in depth info on Guidos' comments on power planes and EMC. With todays fast rise times and high IO count devices, planes can be more advantages if closely coupled with a ground plane (0.1mm dielectric thickness or less) but these designs are often more complex (100 plus pin BGA's etc) than DIY layouyts.
http://eprints.eemcs.utwente.nl/6241/01/Power_tracks_instead.pdf
http://www.radiocad.com/_downloads/PowerPlane.pdf
Have Fun
 
Hahaha I Got it ! Thanks !

Lots of reading for me
I guess as you said, all this is over engineering for such a simple project and small PCB (lengths are so small that I really shouldn't worry about the loops...) also there's no clock or high frequency involved, so you're probably right about having a simple ground plane...

Fred
 
Member
Joined 2005
Paid Member
Hi Lazybutt, I like your design. The groundplane looks good to me. Alternative could be to not have the splits in it but implement one split vertically across the board around C5 location, and connect the two ground planes only there. That would help with the current carrying in the connections.
Another thing, the connection from the drain of the upper transistor to the lower transistor and then output looks thin, and I think you have the space to make it wider.

just my two cents.....
 
Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.