star ground vs. ground plane

[pacificblue]

Decide first, which components you actually use, then optimize the layout for them. Too many options for a certain component means too many compromises.

Then decide, if you want to use planes or not. If you use planes, use them for the V+ and V- potentials as well.

If you don't use planes, in a power supply you want the traces as wide as possible to keep trace resistance (= temperature rise) low. So make the V+, V- and Gnd traces wider up to the point, where they look like planes, but don't pass the planes above and below each other, and keep some distance between them. Something like a mix of your two designs. That means V+, V- and GND will all be on the bottom layer, the V+ and V- planes extend up to the board edges, and the ground plane remains within the limits formed by the V+ and V- planes.

Move the big electrolytics as close as possible towards each other, so that resistance and inductance between them on the ground trace/plane becomes as small as possible.

Don't you need a ground connection at the output? The PCB ground is the reference for the regulators, therefore all components that you connect to them, should reference their power supply ground pins to it as well and it should become your star point for that purpose.

[okapi]

Originally posted by pacificblue
Decide first, which components you actually use, then optimize the layout for them. Too many options for a certain component means too many compromises.

Then decide, if you want to use planes or not. If you use planes, use them for the V+ and V- potentials as well.

For the moment i want to respond to your first two comments. It is definitely true that i have a few to many options. In the version i ordered i have a couple less options than what i am showing in the above pictures. I should mention that i do have a lot of options because it is an experimental board - the final version will just contain the parts necessary for optimal performance. Also, it is only experimental in the sense that i plan to use it to test the effects of various configurations so that I can do some hands on learning. A more experienced person might see most of my tests as rudimentary and consequently a waste of time.

I am having a hard time visualizing how to implement planes for the V+ and V- in addition to the ground. Wouldn't this require 4 different planes: V+in, V-in, V+out, and V-out? Also the pin arrangement of the voltage regulators would require that the planes for V+in and V+out overlap which is not possible with just a two layered board. Would you then recommend having the planes meet near the voltage regulator and then have discrete traces running from the plane to the appropriate pin?

I'll try to address your other helpful comments when i get a chance later today. Thanks for your help.

[FlexQ]

I havent been into this for much more than a year, but i am working as a traineee in a company which makes all sorts of wireless communication links, phones, bluetooth things and so on.

I have been so lucky to have been working with designing a 100W RF generator, for two reasons, there is SO much to learn in designing such a thing, and one gets a good feeling about grounding .

However, this was designed to be a 4 layer print, but never the less.

I was told to find out which was best, star grounding and groundplaning.

Star grounding because i could make the print inhouse for "free" (a frew pennies).

But, i must say that it just didnt work too well.

I thought that it might be because of the high frequencies, and yes, that had alot to do with it. But my most recent pa150 lm3876 amp had the same problems.

I knew where the power came from, but the leads for my small caps just couldent do the job, no matter what i did. So i decided to use 10 times the time to make my design at a 2 layer print, and then optimize the layout for a good groundplane. And i have no troubles with noise of any sort.

So in my experience the groundplane is the best.

But with that said, i might add that, as with all other electronics, it will bee good but never great, if you dont know what you are doing. So if you feel comfortable with star grounding, then do that. But dont discard the other, use the time to learn what the two different ways of grounding has to offer.

In relation to the talk about seperating the signal ground and pwr ground, it is a good idea, i have had a great deal of luck with that as well.

I used a buffer preamp before the 3xlm3876, and the supply for that was as well not directly connected to the pwr supply. I made a DC shorted low-pass filter between them. And that works wonders.

Someone in here who had the same experience?

[Mr Evil]

Originally posted by pacificblue
...but don't pass the planes above and below each other, and keep some distance between them. Something like a mix of your two designs. That means V+, V- and GND will all be on the bottom layer, the V+ and V- planes extend up to the board edges, and the ground plane remains within the limits formed by the V+ and V- planes...

Why do it like that? If you have the ground traces follow underneath V+/V- then you get lower inductance (due to decreased loop area), plus the extra capacitive coupling.

[pacificblue]

Originally posted by okapi
I am having a hard time visualizing how to implement planes for the V+ and V- in addition to the ground. Wouldn't this require 4 different planes: V+in, V-in, V+out, and V-out? Also the pin arrangement of the voltage regulators would require that the planes for V+in and V+out overlap which is not possible with just a two layered board. Would you then recommend having the planes meet near the voltage regulator and then have discrete traces running from the plane to the appropriate pin?

Yes, to all.

Originally posted by Mr Evil
Why do it like that? If you have the ground traces follow underneath V+/V- then you get lower inductance (due to decreased loop area), plus the extra capacitive coupling.

If you prefer it like that, you should probably use planes to start with.

[okapi]

Originally posted by pacificblue

Yes, to all.


If you prefer it like that, you should probably use planes to start with.

Thanks to diyaudio forum member Marce i was made aware of the following article:

Constructing your Power Supply - Layout Considerations, by Robert Kollman

It is a great article and it served to demystify pcb design quite a bit.

On page 4-5 last paragraph it says the following:

"It should be noted that the effectiveness of the ground plane depends upon it being significantly wider than the trace above it. For example, if the ground plane were the same width as the trace above it in Fig. 7, the resulting symmetrical conductor pair has a total inductance per unit length slightly greater than the value calculated by the formula of Fig. 7. However, this total inductance value is distributed so that one half appears in series with each conductor. Thus, the lower conductor is no longer an effective ground plane. When the lower conductor is made significantly wider, the asymmetrical structure causes almost all of the total inductance to appear in series with the smaller conductor, thereby minimizing the impedance in series with the wider ground plane. "


The article also provides a formulas to calculate Trace inductance (Fig 6 and 7). In both cases trace inductance is critically dependent on trace width.

So it seems that the second design i posted, the one with the ground plane on one side and individual traces on the other, with respect to trace inductance, may in fact be the best choice.