Will copper pour help on my single-layer PCB?

I have a PCB which contains one 20x4 LCD, eighteen 12x12 mm push buttons, and three LEDs. This board is connected to an Arduino Mega through a 30 cm long ribbon cable. Now during testing, I found that sometimes the LCD goes blank. In my previous PCB I was not using a ground pour, but if I use a ground pour, will my system be more resilient to EMI noise?

I am working on other aspects as well, but I just want an expert opinion on this to use a ground pour or not on a single-layer PCB.

I am attaching both PCB pictures for clarification: one with, and one without a copper pour:

After reading through all suggestion I have following understanding in my head 1. Transfer VCC and ground lines near LCD interface line i.e. on right side

1. Remove jumper connections on each button lower two pins as they are trans versing copper pour making it less effective.

3.Increase distance between R1,R2 and R3

4.Increase space between LCD control lines and button lines at down right corner.

1. Add more ground lines( I am not sure about that but experts have suggested this)

2. Place connector on top instead of bottom as it will reduce track distance for lcd control and data lines which in turn will make it more immune to noise?

Please comment whether I am in right direction. Two layer is not an option as here in my area they only make two sided pcb in big quantity otherwise its too expensive. Same is the case of china manufacturing

• What LCD? How is information transferred to the LCD (interface type, protocol, timing/frequency, etc.)? Jul 20, 2019 at 13:15
• If you want to use a single-sided PCB only in order to save money, it might not be that much more expensive to get a double-sided one and you can improve the EMI performance. It might even be the same price. Jul 20, 2019 at 14:48
• Your PCB isn't one layer though, you have a two vias and a trace on the other side in the top left... Jul 20, 2019 at 21:09
• @BeB00 Actually it is single layer. That trace is jumper on components side Jul 21, 2019 at 5:00
• @BeB00 china is not an option as it will be still costly and will take much time. I m already very late Jul 21, 2019 at 6:08

7 Answers

A ground pour, by itself, is unlikely to rescue an inadequately grounded board.

A ground pour is not, of itself, a ground plane.

A ground pour is the default for PCB fabrication because it means less copper has to be etched off, a multilayer board ends up more mechanically balanced, and it's more thermally conductive, all good things.

You need to make sure that, without the ground pour, all critical signals have an adequate ground return path. The point of checking this without the pour is that the pour confuses the picture, it makes it very difficult so see what's going on.

Make sure that clocks and strobes have a nearby ground track going from source to sink. Add ground tracks as close as possible to the signal tracks. Make sure that ICs that draw sudden pulses of current have nearby decoupling caps, with short tracking to the power and ground pins. Check that supply current changes don't induce voltages in unwanted places, which generally that means run a ground track with all power tracks.

Perhaps you feel you don't have room to add ground tracking? If there's no room for a ground track, then there's no room for the pour to connect and provide your ground continuity in the right place. Sure, it might connect by going in a big loop somewhere else, but that's not the right place. There is no alternative to providing proper ground continuity in the right place if you want a robust board.

Once your ground tracking is sanitary, then you can add the ground pour back again. If your ground tracking is adequate then it's not really needed electrically, but it won't hurt, and it does all the other good things.

On the other hand, a ground plane is something you design in from the start. It's something you don't cut up with tracks traversing it. It's not something you pour in as an afterthought, after you've routed all the signal tracks. It's the most important conductor on the board, so you put it in first, and look after it as you add the other tracks.

Check AnalogSystemsRF's answer. I told you what you should have done and should do next time, he tells you what you can do now. You'll notice they both involve actually connecting the grounds.

• In your third paragraph Make sure that clocks and strobes... you are describing that everything has to have a ground trace nearby. But a ground fill means there is ground everywhere! Look at the first picture in OP's question. How can something not have a path to ground? How can traces be better than this? I don't understand. Oct 9, 2020 at 12:04
• @PouriaP That quote continues Make sure the clocks and strobes have a nearby ground track going from source to sink. A nearby lump of ground is no good unless it can conduct the return current from sink to source close to the track. That's why a ground fill is bad, it confuses the board and makes it difficult to see whether every clock track does have this tight return path. Check out the 4th paragraph, and in fact the rest of the answer as well. You've heard of things being 'necessary and sufficient'. An unthoughout ground fill is unnecessary and insufficient. Oct 9, 2020 at 14:05
• OK that's exactly what I don't understand. So by going from source to sink do you mean from the GND pin of the component in question to the power supply GND? Oct 9, 2020 at 15:29
• No. I mean when a signal goes from a driver IC to a driven IC, there must also be a conductive ground path from the ground pin of the driver IC to the ground pin of the driven IC, which stays very close to the signal track. The conductive ground path can't take a detour via the PSU ground without trashing a high speed signal. Very low speed signals can get away without this parallel ground path, but few logic signals have the very slow edge risetimes required to be called low speed. Audio would get away with it, but then you have different ground routing issues to worry about. Oct 9, 2020 at 16:25
• @PouriaP Let's put it another way. It is OK if the only ground connection the driver and driven ICs have is a direct route each to the PSU. However, then the signal trace has to follow the route of the grounds, not go directly from one IC to the other. What you want to avoid is a loop of large area between the entire signal current path and the ground current path. With an undesigned ground fill, it's dead easy to have a signal trace hop over a cut in the ground plane that causes the return current to take a long detour away from the signal track. Oct 10, 2020 at 11:45

Ground pours MIGHT help (but like others I have my doubts), but I would be looking at that ribbon cable as a first suspect.

If you changed it out from a 0.1 inch ribbon to a two row connector with a 0.05 inch ribbon (Think old PATA cable) then you could interleave ground with signal, and this I think might help.

I note at the moment that your LCD control lines run up the right hand side, while the LCD ground runs up the left, this is pessimal from an SI perspective. Data and ground should be routed together as far as possible (Also power!), and as the switch matrix is not concerned with either I would move the power and ground pins to be in among the LCD control lines.

On the subject of ground loops, WHO CARES! Current flows in loops (always), you can make it easy for it to do so, in which case little voltage will be developed across those loops, or you can make it difficult in which case much voltage will be developed across the loop, generally lots of small loops beats one big one.

Oh, a detail, but you might want to consider adding some diodes to the switch matrix, it can allow you to handle two switches pressed at the same time more reasonably.

Take 20 pieces of copper wire, and solder the 20 pieces OVER the signals, from GND to GND. In other words, short together some of those floating GND "antennas".

Then retest.

Perhaps add another 20 pieces of copper wire, from GND to GND.

----------- let use compute how bad the GND errors can be ------

Assume a black-brick battery-charger 4" (0.1 meter) away, from 4" by 4" region of the floating Ground Fill pieces. Assume the switching power supply inside the black-brick has 200 volt in 100 nanosecond switching voltage; this is 2 volts / 1nanosecond slewrate. Assume the switching node is visible to the outside world, and causes rapidly changing electric fields.

How much displacement current will be induced into the Ground Fill pieces?

C (parallel plate) = E0 * Er * area/distance ~~ 9e-12 Farad/meter * A/D

with Er = 1(air), Area = 0.1m * 0.1m, and Distance = 0.1m

C = 9e-12 * 0.1m * 0.1m / 0.1m = 9e-12Farad.meter * 0.1m = 0.9pF

C ==== 1pF approximately

I = C * dV/dT = 1pf * 2v/nS = (1nF * 1milli) * 2v/nS and the NANO cancel

I = 1milli * 2v = 2 milliAmps, at the black-brick switching rate frequency

Now we need to compute the GND--to--GND resistance. The best possible is about 1 square of copper foil (0.00050 (actually 0.000498 at 25 degree C) ohms). With 20 or 40 pieces of wire connecting the floating pieces together, the size of the wires and the length of the wires also affects the GND--to--GND resistance, but the wire diameter will be thicker than foil, and your fill-gaps are 3milliMeters (1/16th inch), so we'll just assume 2 squares of foil or 0.0010 ohm (the resistance is very sensitive to temperature: 0.4% per degree C).

What will be the voltage difference between one location on the GND and some other location on the GND? use Ohms law: I * R

Assuming the resistance is 0.001 ohm, and I is 0.002 amps, the voltage is just I * R, or 2 milli milli or

2 microVolts (DC low frequency)

Should we allow for inductance? sure. With the various parallel paths thru the various pieces of wire, assume the Inductance from point A to point B is 10 nanoHenry (a solid sheet of copper is about 1 nanoHenry inductance. I welcome better estimates, and even a formula). The Z (impedance of 10nH at 5MHz, or 1/(2*100nanoSecond)) is +J 0.031 ohms. Z (1nH at 1GHz) = +j6.28 ohms. Z (1nH at 1MHz) is 6.28/1,000 = 0.00628 ohm. At 5MHz, the Z is 5X larger at 0.031 ohms. Notice we don't need a calculator.

What is the voltage? I * Z, or 2ma * 0.031 ohms, = 0.062 * milli, = 62 micro Volts.

Thus we predict some (small, but not ZERO) voltage from Ground to Ground, as currents flow thru those 20 or 40 pieces of wire you added between the floating Ground Fill pieces.

62 microVolts (AC, at 5MHz)

• On multi-layer boards, vias would do the trick, making them a less labour-intensive option.
– Mast
Jul 20, 2019 at 18:40
• Will not these creat ground loops? Jul 21, 2019 at 6:02
• If you have charge upsets that sustain loops, then these newly added GND--to--GND paths will reduce the point-to-point differences. Excellent question. Can we compute the GND--to--GND voltages? yes. Use Ohms Law. If you have 1 microAmps of GND--to--GND charge movement from 60Hz electric fields, and the GND--to--GND resistance is 0.001 ohm (which is 2 squares of standard-thickness copper foil, as 0.00050 ohms per square), the voltage GND--to--GND is 1uA * 0.001 ohm, = 1 nanoVolts. This is not ZERO volts, but for a 16-bit ADC with 3.3 volt full-scale or 50uV Vquanta, the 1nV is 50,000X smaller. Jul 21, 2019 at 9:29

Your LCD probably goes blank because of faulty contrast trimpot. Better to use fixed resistors instead. Grounding is unlikely the problem

You can clean up the tracks on those switches.
The bottom left and right pads are joined internally as are the top left and right. You can run a simple track straight up between (for example) B1, B4, B7 and BX. Add joins to ONE pin on each switch and you get a cleaner layout.

Avoid making "islands" with your ground pour. Every area needs to connect. You could even spread R1, R2 and R3 to ensure a better pour between them.

Since the LCD only blanks sometimes, and I ASSUME this isn't for mass production, this pour Might be enough to keep you going. I'd still advise a double sided board as a better solution.

To fight EMI remember that current is a two way concern. If you are limited to single sided, rout return paths in close proximity to each other.

Some low value, series resistors in signal paths make the circuit less likely to radiate. And every signal that enters or leaves the PCB should pass through a resister before it goes to an IC.

• Adding resistor in series is novel idea for me (or may be I am novice) but please could you further explain it Jul 30, 2019 at 11:22

I don't know if you're going to mass produce things, but if I were prototyping I would use a double-sided board, spray one side of the board with resist, this would be the ground common, include pads for ground connections on the circuit side, and use primitive thru-hole soldering.

You would do best dividing the ribbon cable into two cables, the low frequency on one group, the HF on the other.