On a board with separate analog and digital ground planes connected at one place, the connection is often made with an inductor. How is this inductor chosen? Obviously it has to be able to handle enough current, but what other factors are important?

I'm more interested in the type of inductor rather than the value, since I would expect to try different values.

  • 7
    \$\begingroup\$ 0 Henries is a good value. Connecting grounds with inductors means they won't be connected at high frequencies, so they aren't grounds anymore. This does not sound like a good idea. \$\endgroup\$ Jul 3, 2012 at 14:19
  • \$\begingroup\$ The whole idea is that you don't want them to be connected at high frequencies. It's supposed to keep noise from the digital section away from the analog one. \$\endgroup\$ Jul 3, 2012 at 14:53
  • 9
    \$\begingroup\$ Yes, I've heard this a few times but it doesn't add up. Connecting true grounds isn't going to spread the noise because ground is the reference, not the noise. If you want to keep high frequency return currents off the analog ground, connect them in one place with the right topology, not try to block high frequencies. Playing games filtering grounds will cause more trouble than it will solve. \$\endgroup\$ Jul 3, 2012 at 15:14
  • 2
    \$\begingroup\$ @OlinLathrop Hallelujah! Truer words have not been spoken. I hate having to deal with designs that have deliberate inductances in the ground. "But it used to work..." \$\endgroup\$ Jul 3, 2012 at 17:03
  • 3
    \$\begingroup\$ I never realized how actually true the statement is that the reverse current in the ground plane wants to flow right under the conductor carrying the forward current. Until I saw this little video: youtube.com/… You might want to forward to about 12'00" \$\endgroup\$
    – jippie
    Jul 3, 2012 at 19:56

3 Answers 3


Another school of thought is to forget the inductor and split ground plane. Instead use a solid plane, but use careful placement and routing to ensure the digital/analogue signals stay in their respective portions of the PCB.


According to the figure below, you can see (for high speed signals) most of the return current flows very close to the trace (x is distance from centre of trace, h is trace height above plane):

Current Flow

No time to go into more detail right now (will try and add more later) but here are a couple of excellent links on the subject:

Henry Ott - Mixed Signal Layout
TI - High speed Layout Guidelines

  • 4
    \$\begingroup\$ One way to get these values to basically 100% is to make separate nets for each of the sub-grounds, then connect them to the main ground plane in only one place. The main ground plane current then only carries the unavoidable return currents between the functional blocks, but not any of the potentially nasty currents within a block. \$\endgroup\$ Jul 3, 2012 at 16:09
  • 1
    \$\begingroup\$ +1 for linking to Henry Ott's article. Jeanne, you should read that. \$\endgroup\$ Jul 3, 2012 at 16:16

Ideally your ground should be 0 V everywhere, so a voltage drop due to any impedance is out.

Olin notes that connecting grounds with inductors means they won't be connected at high frequencies, so they aren't grounds anymore. That's correct. But if you completely isolate your digital and analog part for high frequencies you won't need a ground return path for them either. This makes only sense if you block the high frequency noise in all other connections. Power supplies and signals. I've used Murata BLM noise suppressors for this; a BLM18PG221SN1 has a DC resistance of 100 mΩ maximum, and an impedance of 220 Ω at 100 MHz.

enter image description here

Combined with a capacitor you get a second order filter which will deal with that microcontroller noise. The low resistance means a minimum voltage drop in supply voltages.

If you can keep HF noise away from the analog part you can couple both grounds directly, but at 1 point.

When I worked with Philips Audio wired ferrite beads were sometimes used to connect digital and analog ground:

enter image description here

DC resistance is in the milliohm range, but like Olin says they will offset ground for HF if you allow it to pass to the analog side.


its better to have one solid ground plane and partition your board layout than split grounds

  • 1
    \$\begingroup\$ Not in all cases its not, sometimes it is better to have two. In most designs I have encountered it is better to have one. It also depends on many other factors. If your main ground is already noise or has a large common mode noise source, it may be advantageous to having two grounds. \$\endgroup\$
    – Voltage Spike
    Jun 9, 2018 at 19:19
  • \$\begingroup\$ If the board has mixed SMPS supply and analog and digital sections the ground plane must be split. \$\endgroup\$
    – user105652
    Jun 9, 2018 at 22:53

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.