# Is GND plane required on only one side of the board?

W.R.T this case…if I place the tracks(Green) on the other side making it red, i might be able to cover up the board with GND place on one side but it may cause issues on the other side but is it required to make GND plane equal enough on the other side?

A GND plane is only usefull if your current return path needs a gnd plane.
As you have low side switches. A gnd plane will not be of any benefit in your case.
In your case a v+ plane might be more useful.

In other words. If there is nothing on your board that connects to the gnd plane, it is useless and does exactly nothing except maybe reduce the amount of edging fluid needed or the time needed for milling the pcb.

A good read for emc aware design would be this document by infineon.
http://www.infineon.com/dgdl/Infineon-ap2402633_EMC_Guidelines.pdf-AN-v03_05-EN.pdf?fileId=5546d46255dd933d0155e32392f1090e

In more complex pcbs one normally has both a v+ plane and a gnd plane on inner layers.
(If there is more than one voltage supply there can even be multiple v+ planes)
This allows short current return paths without the need for the designer to think about it for each trace they lay down.

Also having v+ and gnd planes on inner planes creates a very good capacitor between these two.

1 Like

Now it does. Pin 7 will have GND

Yes gnd is connected to the plane. But there is no current flow if only one device is connected to a trace or plane.

Do you know what i mean with current return path?

1 Like

you shall explain about current return path

I try to explain it as simple as possible but i fear you might need to read some basic literature.
(I don’t know of good English literature that explains the basics. I learned that in German.)

Each electrical signal is in essence moving charge. This moving charge is called current. (In metals the moving charges are electrons. Current is charge per time instance.)

This current is driven by a potential difference at the so called source of the current. (A potential difference is called voltage.)

For a current to flow there needs to be an electrical connection from the positive potential to a negative potential. Electrical engineering is the art of controlling this current path in such a way that the current does work for us.

The current path is the exact path a current flows through in this process.
In direct current applications this path is determined by the path of least resistance. (ohms law) In alternating current applications this path is determined by the path of least inductance (simplified calculations can be done using the complex inductance. It also helps in understanding some of the effects that arise in high frequency applications.)

The goal of good pcb design is that the loop that is created by the current flowing through the pcb has the smallest possible area.
Here the law of induction comes into play. The self induction as well as the possible couple induction to nearby loops is in part determined by the area of this loops.

In most cases designers are concerned about the current return path because the first half of the current path is well defined by traces.
A copper plane for the “return” path enables the current to flow back directly under the trace where it came from, thous reducing the area of the created loop. (it is not always the gnd plane. In high frequency applications the concept of a gnd makes no sense.)

In your case no current will return through your gnd plane because this part of the current is defined by the traces you created. (otherwise you are not able to switch this currents.)
The only thing you could do to reduce the loops is to give the current freedom in the positive side of the current path. That’s what copper planes are there to do. (but they only really work if they are not split up by anything. Which means you would need more layers.)

In a two layer pcb one could for example create a good plane by having all horizontal connections on one layer and the vertical connections on the other layer. This is only a compromise and needs a lot of work. (changing layers creates high impedances.)

So what can you do to make your pcb better. (especially important for future pcbs) Not everything i tell you here applies for your current project!
First identify the path the current takes for each signal. (yes for each of them.)
Identify signals that are critical.

• Signals with high switching frequencies and or fast switching times.
• Analog signals.

Identify a voltage potential that is shared by most of your signals on this pcb. (in your current pcb this is the potential all of your transistors share. In most other pcbs this is gnd.)
This potential is a good choice for a copper zone. (If you have multiple layers, you have more possibilities here.)

Place your devices in such a way that the current paths for this critical signals is reduced. after you are happy with the placement make a first routing pass. (start with the most critical signals first.)
During the routing process you will find that some devices could be placed better. Move them and start over with the routing of the pcb.
Repeat this until you are happy with the result or the deadline comes.

I hope this gives you a good starting point for your learning process.

3 Likes

Very good lesson! Not related to Kicad, I mean, layout tool independent, but useful and excellent abstract.

How to decide on this?

this much i have understood, the importance of current return path.

Not split up by anything means? the spaces in between while laying the GND plane?

I have understood the importance of the GND plane but am not able to figure out why my above circuit doesn’t require it? the transistor relation is also something I didn’t get.

This is given by your display. Also in most cases it is easier to have low side switches because than you can use n channel fets in common source “mode”. (I don’t know a better word here.)

If i remember your circuit correctly you have 4 high side switches to select the digit and 7 low side switches to select what led’s of this digit should be on.

As the low side switches are not part of your pcb but are on the pcb your pcb connects too there is no common gnd.
There is only a common v+ (the common line of your high side switches.)

Here a simplified version of what you pcb looks like. (not all led’s of a 7 segment digit shown, resistors removed, not all digits shown, gate connections not shown)
This might make it more clear.

1 Like

the 13 pin on the connector connects all the emitter of the transistors so should the plane be connected to that pin and will that be a better return path?

Jup that’s the one i meant up in my long explanation:

Yes i know current return path is not really the correct word in this case because it is the more positive signal. (but electrons flow toward + anyway so it might be correct if you think about it this way.)

oh okay…now i understand this a little more clearly. You mean the tracks I laid here are acting as return paths?

and the plane that shall be connected to the emitters will be the plane through which current shall move first? But how will the current get direction then?

But how to keep all these in mind before laying out the tracks. This shall make me afraid of laying tracks I mean with so much to consider, every track will have to be minutely thought of. time consuming then ?

I’m not sure what you mean by that.

But maybe this will help:
Current always flows from the more positive to the more negative electrical potential (note 1).
In most cases we define the most negative potential to be our 0 and call it GND. If we do that we can call our positive potential for example +5 Volt.

Also LEDs and diodes only allow current to flow in one direction. This means you can not simply change your voltages around and expect the circuit to work.

(note 1): I’m speaking of technical current direction here. Electrons flow the other way round. This is because the positive potential was defined before science know that in metals electrons are the moving charges. (The electron itself was found much later.) https://xkcd.com/567/

1 Like

That’s why humans are still better at this task then computers. If it would be easy you would not have a job.

3 Likes

There’s actually far more to it than you yet realize. Your circuit is very basic, although you will be mulitplexing this display it will be at such a low frequency that you can view this circuit in terms of it’s DC characteristics only. So basically the tracks you route will determine the paths along which current will flow. As switching frequencies increase things get more interesting.

3 Likes

Interesting ! Hah !

Is this video clip a parody, or a (almost) contemporary expression of a timeless cultural theme?

To my international friends on this Forum, I apologize for interjecting a uniquely American folk legend.
(See John Henry (folklore) - Wikipedia )

To my friends under age 50 on this Forum, I apologize for the topical references to things from the 1950’s and 60’s. I stand ready to explain them to those who were born too late.
( Or see Tune o’ the Day | Mr. Write's Page )

Dale