How to correctly design ground planes simple circuit PCB's?

Question

I'm a little new to PCB design and could use some help figuring out the best way to make this very simply PCB that I plan to connect to the back of a custom led light sign that I'm making. The circuit is simply a bunch of LED strips that all have the power and ground connected in parallel:

^{simulate this circuit – Schematic created using CircuitLab}

Here's what I've drafted up in Kicad, the wide placement of the components is necessary as I need them to span the whole 15" sign:

I've been reading a lot online about putting ground planes in circuits and I'm hoping I can get some concepts clarified.

1. Are ground planes necessary in all circuits? I tend to design what I think are simpler circuits, that rarely have many signals in them, which I believe is a reason for using a ground plane
2. Is a ground plane worth having in this circuit? Or due to the sparse spread of components is it better to simply have traces? Does that save on copper?
3. Do you need one larger via for the ground plan to connect to the jack or would multiple small ones be better?
4. Why do SMD components not seem to connect to the ground plane, could they not just move the metal through the layers from the top?
5. Will through hole components touch every single layer of the board? I'm concerned that if I make a positive plane and negative plane the thru components will link the two?
6. Would having a positive plane and ground plane in this circuit be worthwhile? Or would it be better in to simply have a one layer board with only traces to positive and ground
7. Does the unique quality of this circuit—in that it only contains connections to positive and negative—allow the PCB to be designed in a way that is simpler/better than a circuit that contains more than just positive and ground
8. Does the fact that this circuit is <3A, or the amperage in any pcb circuit, need to be considered when deciding whether or not to include a ground plane rather than traces?

I understand this is a lot of questions, and answers to one or many(or all!) would be very helpful. Many thanks.

Answer 1

1. Are ground planes necessary in all circuits?

No, it is possible to design a PCB without a ground plane. Ground planes become more of a necessity when:

• Dealing with large amounts of heat (the plane allows for heat to spread out across the board to reduce hot spots).
• Noise shielding.
• High speed signals (the return current for a trace passes in the plane under the trace).
• Tight routing situations.

The primary down side to a plane is it makes it more difficult to hand solder components, since the plane wicks away heat.

2. Is a ground plane worth having in this circuit?

No, but it isn't hurting anything. Two layer PCBs are made by starting with fiberglass (or some insulating material) with copper on either side. Then the spaces between traces are removed by etching or mechanically routing. In theory, removing copper takes effort, so the board should be cheaper with a ground plane (in theory).

3. Do you need one larger via for the ground plan to connect to the jack or would multiple small ones be better?

Either is fine. A via with a 1 mm diameter drill will carry 3 A:

but so will two vias with a 0.3 mm diameter drill:

For high speed circuits, it's better to have multiple vias to reduce the inductance.

4. Why do SMD components not seem to connect to the ground plane, could they not just move the metal through the layers from the top?

I'm not sure if I fully understand the question, but surface mount components typically connect to ground planes in multiple places. Here is an example with the red circles being vias to a ground plane:

When dealing with tight routing, high speed traces, or noisy enviroments, vias are sometimes placed in the pad of the surface mount component (via in pad).

5. Will through hole components touch every single layer of the board?

For through hole components the fabricator puts a a circular pad on each layer (top and bottom for two layer), drills through all the pads, and plates copper in the hole (similar to how vias are made). You can choose to connect your traces to that pad, or not. For inner layer planes, copper is removed between the through hole pad and the plane (assuming they are different nets such as 5 V and ground).

6. Would having a positive plane and ground plane in this circuit be worthwhile?

For this application, you can route the whole thing with traces, and ground planes are not needed.

7. Does the unique quality of this circuit—in that it only contains connections to positive and negative—allow the PCB to be designed in a way that is simpler/better than a circuit that contains more than just positive and ground

I'm not sure what you are asking.

Does the fact that this circuit is <3A, or the amperage in any pcb circuit, need to be considered when deciding whether or not to include a ground plane rather than traces?

Use 2.5 mm wide traces for 3 A current:

At some point the traces become so wide it's easier to deal with a ground plane.

Answer 2

Are ground planes necessary in all circuits?

No, you can use a simple copper wire as a ground. The problem with this is it increases resistance and inductance, the smaller the copper wire or trace, the more resistance it has.

Is a ground plane worth having in this circuit?

You can estimate/calculate the voltage drop through the ground by using a calculator such as saturn PCB toolkit, or you can estimate it yourself. The resistance through the ground will create a voltage, let's say the ground is 100mΩ and you have a current of 10mA, the ground resistance will raise the voltage by V=IR or 100mΩ10mA=0.001mV which isn't much for most applications, if you had 100mA, it would be 10mV and 1A would be 100mV. If you have a switching load this ground 'bounce' could create issues or flicker in LED's. The resistance also creates heat in traces, for low current's it's negligible, for high currents over 1A you may have an issue.

You won't save anything if your manufacturing this board at a PCB house, you will save a few pennies if you build the board yourself and recover the etched copper solution.

Do you need one larger via for the ground plan to connect to the jack or would multiple small ones be better?

Usually one size via is better with multiples, but it depends on what your PCB manufacturer charges, with most designs unless you have hundreds of vias there is no addition charge.

Why do SMD components not seem to connect to the ground plane, could they not just move the metal through the layers from the top?

You use vias to connect layers, avoid via in pad unless you really need to to save space, it creates an addition charge at most PCB fabs as you need to plug them to avoid issues with SMT soldering during reflow.

Will through hole components touch every single layer of the board? I'm concerned that if I make a positive plane and negative plane the thru components will link the two

Yes, the software should not connect the copper pours/planes if you have setup the DFM right

Would having a positive plane and ground plane in this circuit be worthwhile? Or would it be better in to simply have a one layer board with only traces to positive and ground

Depends on what your costs are with manufacturing, a one layer board is cheaper, most places only offer 2-layer minumum. Choosing to do a copper pour/plane for ground or power is up to you, pours lower resistance but take up space.

Does the fact that this circuit is <3A, or the amperage in any pcb circuit, need to be considered when deciding whether or not to include a ground plane rather than traces?

If you are dealing with over 1A, you will need to consider heating in the trace and the resitance of the trace as described above.

Answer 3

Are ground planes necessary in all circuits? I tend to design what I think are simpler circuits, that rarely have many signals in them, which I believe is a reason for using a ground plane

No, not for all circuits, but here you are trying to make what is basically a cable, so you will need a lot of copper. Make the top all +12 and the bottom all ground.

Do you need one larger via for the ground plan to connect to the jack or would multiple small ones be better?

If you have a lot of current it is a good idea to use both larger vias and perhaps several in parallel. KiCad has a calculator you can use to see what you need:

Why do SMD components not seem to connect to the ground plane, could they not just move the metal through the layers from the top?

Surface mount components mount to the surface, so no contact to lower layers. You have to add vias if you want to connect to lower layers.

Will through hole components touch every single layer of the board? I'm concerned that if I make a positive plane and negative plane the thru components will link the two?

KiCAD will only connect it to layers that you indicate in the schematic.

Does the fact that this circuit is <3A, or the amperage in any pcb circuit, need to be considered when deciding whether or not to include a ground plane rather than traces?

Yes, the higher the current the more advantageous the use of planes.

Answer 4

1. Are ground planes necessary in all circuits? I tend to design what I think are simpler circuits, that rarely have many signals in them, which I believe is a reason for using a ground plane

No! definitely not. Whenever you re on a two layer board, power plane aren't really an option. That being said, at the end of the design, it might be a good practice to pour a ground plane in the unused area.

Is a ground plane worth having in this circuit? Or due to the sparse spread of components is it better to simply have traces? Does that save on copper?

That's definitely not useful to have a ground plane in your circuit. Even with a simple MCU, it is often not required. It is still better to have a plane or polygon than trace because they are less resistive, but I wouldn't worry about it. It doesn't really save any copper to have or not ground plane. The manufacturing process is the same. A full copper foil is placed then etched to remove the area. It could be argue that it is better to not remove copper since the acid will last longer but I doubt it is significant.

Do you need one larger via for the ground plan to connect to the jack or would multiple small ones be better?

Several smaller vias is always better. For plane or for traces.

Why do SMD components not seem to connect to the ground plane, could they not just move the metal through the layers from the top?

Not sure I understand your question. But, if your question is why don't we just lave a solid pour with only some traces, the reason is that you need thermal relief to solder. It is more an issue with SMD component then TH, but both should be thermal releifed.

Will through hole components touch every single layer of the board? I'm concerned that if I make a positive plane and negative plane the thru components will link the two?

Yes they will have access to all layers if they are platted. Your software should be smart enough to disconnect them from the top/bottom plane if the connection shouldn't be made.

Would having a positive plane and ground plane in this circuit be worthwhile? Or would it be better in to simply have a one layer board with only traces to positive and ground

Honestly, on that board either won't make much difference. It is better to use planes because they have better resistance in general, but in this instance, it won't make much difference. I think it would be faster to route it with plane.

Does the unique quality of this circuit—in that it only contains connections to positive and negative—allow the PCB to be designed in a way that is simpler/better than a circuit that contains more than just positive and ground

I wouldn't say better, but for sure simpler. Since you can have 1 layer per net!

Does the fact that this circuit is <3A, or the amperage in any pcb circuit, need to be considered when deciding whether or not to include a ground plane rather than traces?

Order of magnitude should always be considered. Especially when you are using smaller width traces. You can find online calculator at first but soon you'll just have some guidelines in head and not really calculate them anymore (unless they are unusual). 3A is not insignificant. I would have to use a calculator to ensure the trace can handle it.