I have a PCB (let's call it PCB #1) that has a Li-ion battery as its power source, sourcing 12V to 17V. The power from the battery is used to step down to 6V using a buck converter on PCB #1. A cable connection sends the input power (12V-17V) to the second PCB (let's call it PCB #2). The 12V-17V is regulated to 12V using a non-isolated DC-DC converter. Both the 6V from PCB #1 and the 12V from PCB #2 are sent (using cables) to the third PCB, PCB#3.

Aside note: PCB #1 and PCB #2 are "set in stone" and cannot be changed. enter image description here

Update: added the note regarding 5V DAC outputs.

A 5V DAC sends two outputs to the 12V circuitry (used as control signals for two HV DC-DC converter modules).

My question is whether the 5V return and 12V return on PCB #3 should be joined together? If I do join them, would that not create a ground loop?

Currently I have them separated and I have a copper pour for each. The 12V return is shown in the top image as light green; the 5V return is shown in the bottom image as dark green.

enter image description here enter image description here

If they should be connected, should I:

  • (a) simply join them together and instead of having GND-12V and GND-5V, I'll have GND?
  • (b) join them at one spot using a low-impedance connection, i.e. using a 0 Ohm resistor or a jumper?
  • (c) join them at one spot using a resistor? (I have personally never done this but it has been done)
  • (d) join them together, but keep them separate with a slit in the ground pour/plane?
  • (e) should I leave them as is, i.e. separate from each other on PCB #3?

Thanks in advance.

  • 1
    \$\begingroup\$ Simply joining them is likely to be the best. Have sufficient decoupling capacitors such that current from board #3 to power supplies are mostly low frequency. With DACs supplying signals across the voltage regions, you want to have a solid ground reference between them. If the links between the power supplies and board #3 are noisy (not saying it would be, with limited info the guess would be from DC-DC converter), with sufficient decoupling (there is a reason for this name) capacitors on board #3, you can put ferrite beads between one or both of the power supplies and board #3. \$\endgroup\$
    – rioraxe
    Commented Apr 9, 2016 at 0:01

2 Answers 2


In any circuit, current has to return back to the source and it will take the lowest impedance pathway to do so. So lets look at your circuit, you didn't really specify how the 3rd board functions which is important. There are problems that you will run into which may or may not be a problem for you. There is also no information on secondary cables that might be attached to the board.

If you are planning on sending this design through regulatory compliance testing or an FCC cert, you will have potential problems. If you have sensitive analog electronics, this design will also have potential issues. If you don't plan on any testing, as long as you don't have too much ripple you should be mostly fine.

1) If you connect the boards you will form a ground loop with your cabling with the grounds, to reduce this problem you will need to minimize the loop area AND reduce the impedance between boards 1,2 and 3 as much as possible. This means keeping the cables short, and the distance between the boards close. Use a thicker gauge wire to keep the impedance between the boards lower (to reduce common mode noise).

2) If you don't connect the grounds you will have a nice dipole antenna.

There are also some things you can do to mitigate these problems, to prevent high frequency noise from getting to the DC to DC converters and onto your board, you could use a ferrite on the cable (increasing the inductace and thus increasing the high frequency impedance)

Another way to test this is to stitch the two ground planes together in several places with 0 ohm resistors, if one way works better than the other you can leave them or remove them. The more resistors you have in more places the better off you will approximate a connected ground plane. This is not exactly the same as having a sold ground plane as it will add a few nH's of inductance and mΩ's of resistance between the planes but it works great for testing.

EMC is an art, because most of it depends on parasitics and circuit elements that are difficult and impossible to measure. Something that might work for one design may not work well for another because of the small details. A good way is to plan for this in the design phase and come up with good testing methods.

  • \$\begingroup\$ The 3rd board creates a high voltage output. The 12V circuitry mainly powers the HV DC-DC converters and a few relays. The 5V circuitry controls the HV DC-DC converters. There are a few analog ICs that measure the high voltage feedback. 1) The boards are all close to each other. PCB #2 is mounted on PCB #3 and PCB #1 is a few inches away. The connection between PCB #1 and the other two PCBs is a 20-pin ribbon cable. 2) Should I prefer having a nice dipole antenna over ground loops? I do not have too much space and putting several 0 Ohm resistors would not be easy to do. \$\endgroup\$
    – CuriousCat
    Commented Apr 8, 2016 at 21:01
  • \$\begingroup\$ Like I said, it will come down to testing, there are too many factors at play. If you are using this in a product, you will want to do that and see what works best for your application. If your not, then do your best. 0603 resistors don't take much room, if you have to move to 0402's. There are also solder bridges that you could use on the pcb google.com/… \$\endgroup\$
    – Voltage Spike
    Commented Apr 8, 2016 at 21:15

If the logic circuitry is completely separate between the 5V and 12V sections as you have drawn them, then they do not need to share a common ground. You only need a common ground if you use the 5V section's output as an input to the 12V section or vice versa.

  • \$\begingroup\$ I forgot to add that there are two 5V DAC outputs that are sent to the 12V circuitry. I have updated the image and the text. Thanks. \$\endgroup\$
    – CuriousCat
    Commented Apr 8, 2016 at 20:41

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.