[walangalam]

I'm designing a Gilmore dynalo Power Supply board that I plan to put inside a Hammond 1455. The board will just be single sided. It will accomodate all the parts, including an amveco 25VA toroid.

Should I use a ground plane or just try to do a single point ground? If ground plane, do I plane the whole board or just parts of it?

Thanks in advance.

 

[amb]

You cannot do a "ground plane" when the board is only single-sided. With such a board the best you could do is a big ground trace that run around the other traces. A ground plane typically refers to a separate layer of the board, dedicated to ground only. Sometimes portions of the ground layer needs to be carved out to accommodate other "jumper" traces that cannot be routed efficiently on the regular circuit layer.

 

[skyskraper]

the work has already been done for you.... http://www.gyraf.dk/gy_pd/calreq/minipsu.pdf

 

[walangalam]

yes, thanks amb. Thats what I meant - a big ground trace that runs around all the traces thats essentially unbroken.

Is it better to do it this way than to have a single point where all the grounds meet?

 

[amb]

There is no simple answer to that. It all depends on the layout. As you are probably aware, as long as there are currents flowing through the ground traces, there is going to be a small amount of voltage difference between various points of the ground path because the impedance of the copper in the traces isn't zero. The solution is to minimum that impedance in order to minimize that phenomenon.

A separate ground plane layer is most convenient because there is a lot of copper for the lowest impedance, and parts that need a ground connection can be tied to the ground plane right where it is. Moreover, the ground plane serves as an electrical shield against external interference (although for a power supply this is of minimal importance).

Single point grounding is basically "star grounding" applied to printed circuit layout (where each part that need to connect to ground has its own path, leading to a common ground point that is used as reference). In reality it is usually unfeasible to design a PC board with so many separate ground paths, for space and routing reasons. Also, if any branch of these paths is long, then the trace impedance will cause voltage to be developed, which is undesirable.

For single layer boards, you can arrange the parts that need to go to ground such that they are located near each other, and then have a large ground copper area (or a plane) to tie them all together. This would then essentially be the same thing as single point grounding done right.

 

[Syzygies]

Amb, thanks for the clear explanation.

What little I know about this is from datasheet recommendations (some of them are epic novels). It's enough to convince me of the merits of home etching double-sided, make ground planes a habit. However, you've covered the "real part" of impedance, resistance, I'm more confused about the "imaginary part" of impedance, inductance and capacitance.

I read that one uses a ground plane in places on a circuit where one wants to minimize stray inductance (same reason one doesn't want vertical resistors), while one wants to avoid a ground plane in places on a circuit where one is more concerned about stray capacitance. I read in examples people tend to put input signal paths or very sensitive IC's in the "avoid ground plane" category.

Can you clarify this point? Is it an art that takes a scope and years of experience, or are there some reliable rules of thumb?

 

[amb]

Yup, a ground plane could be bad around certain portions of circuits, especially where the impedance is high and the speeds are fast. For example, near the input pins of a precision opamp, you'll want to avoid a ground plane because that would cause stray capacitance between the inputs and ground. Such capacitance wreaks havoc with the stability of the opamp at very high frequencies.

In the M³ amplifier PCB layout, you'll notice that the ground plane avoids coming too close to the opamp input pins.

The converse of the capacitance would be the scenario of a very long ground trace. High speed, high frequency signals traveling through such a trace will be subjected to its inductance, which is clearly not desirable. Having a ground plane minimizes the length of ground paths and lowers the overall impedance of the ground circuit.