I have 3 separate grounds in my project:

  • AGND - Analog ground is very quiet, very small relatively smooth currents
  • PGND - Power ground used for power bypass caps and power supply related circuitry is less quiet
  • DGND - Dirty ground for digtal, led drivers, relays and things that cause horrible fast transient spikes and high current spikes

These grounds run over separate traces / wires back to a "star" on the power supply board.

Q: If I make a ground plane area that is DGND (the "dirty" ground), is that more or less likely to emit noise that could be picked up by surrounding circuitry as opposed to making the DGND circuitry regular traces and using another ground like PGND for the ground plane?

Generally we think of ground as being a low noise low impedance path. But if it's actually really noisy like a "dirty" ground that can see enough current to cause 100 mV spikes relative to a regular "quiet" ground, is that suitable for a ground plane or will putting noise into a big plane cause more harm than good?

  • 1
    \$\begingroup\$ Sounds like your missing some bypass capacitors on the power feeds, and/or the ground traces need to be wider so as to have a lower impedance. When ground planes go to another layer, stitch them together with many small vias. Have you checked for these issues? \$\endgroup\$
    – user105652
    Commented Jun 24, 2016 at 17:00
  • 1
    \$\begingroup\$ Yes, in theory if the current source is bypassed well enough and impedance of the trace / wires are large enough, the transient spikes should be eliminated. But in practice this is simply not the case. Specifically, I have an LED driver that is so fast that no amount of bypassing eliminates the noise. I played around with it for a whole day trying different things and it didn't even really make much of a difference. Take the LEDs out and works great. LEDs in, major noise. So I use a completely separate "dirty" ground. That of course fixes it. \$\endgroup\$
    – squarewav
    Commented Jun 24, 2016 at 17:40
  • \$\begingroup\$ Voltage and noise can only exist from point to point. So a GND plane can be "noisy" only if it has large and varying currents traveling on it. There is a good chance that your situation will be much improved by simply creating a single ground plane (instead of 3) that is as low-impedance as possible. There is no way you will get 100 mV from point to point on a copper plane. Use intelligent placement of components to minimize the distance traveled by high-currents on the plane. Consider adding extra copper and vias to give higher GND currents an easy path. \$\endgroup\$
    – user57037
    Commented Jun 25, 2016 at 17:17
  • \$\begingroup\$ What is your project? I mean, do you have low voltage signals with high series impedance outputs? If not, you probably do not need an analog ground. Separating PGND from digital GND also seems like a bad idea if your bypass caps are connected to PGND. Bypass caps need to be as close as possible to the IC pins they are bypassing, and connected to the exact same power net. Otherwise it is almost pointless to have bypass caps. \$\endgroup\$
    – user57037
    Commented Jun 25, 2016 at 17:22

2 Answers 2


The spiking that you are seeing on the ground plane is actually a voltage difference due to current running through the return path from your driver. Large, high speed changes in current create a voltage difference for various points in the return path due to its inductance. To keep the noise from bleeding over into your other circuitry, you can try the following approaches:

  • Do not place the dirty ground plane in places where there is no current path. A common error is to make this ground plane the entire board area. This creates a large capacitor plate in areas where there is no current, and non-current-carrying portions of the ground plane have the voltage spikes from the adjacent current path.

  • Keep the quiet stuff and their traces away from this ground plane. Traces on a separate layer can be capacitively coupled to the plane.

  • Watch out for loops. Your current path to and from the devices with the high frequency, high current ideally should be close together and parallel to reduce the loop area and associated induced voltages. Best to have the power going out and coming back from your source be close together and parallel to the extent possible.

  • Keep the high current runs short.

Hope this helps.


That was a smart move to create a'dirty' ground for the LED's. A better term wound be 'high-current' ground for devices like LED's, relays, etc. A good way to quiet these type of power feeds is to combine series inductors >100uH with large value capacitors >1000uF.

Keep the independent ground-that was a smart move, and it would be the return path for the large value capacitors I mentioned. Having a quiet high-current power feed prevents EMI and cross-coupling noise off of your other power feeds. This should improve what you already have in terms of noise and ripple.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.