How can ground loop be avoided when connecting two system with same ground. This happen in PC with SATA cable or PCIe Card with separated power cable.

My System

  • Board: I have two pcb each with a ground plane. The board #1 is powered up by a battery. and through board #1, battery connected to board #2 via two wire (battery V+ and V-).
  • receiver : receiver is WF111, a wifi module run @50MHz with SDIO
  • Transmitter: Transmitter is ZYNQ-7000 a Cortex A9 processor
  • Power: the processor is powered with LDO #1 (simplified) and WF111 through LDO #2(again simplified).
  • Signal: the signal between transmitter and receiver connected with a FFC cable between two boards. enter image description here


Sending gnd for current return path as suggested here, will create big ground loop and will act as a big antenna. So what you suggest.


2 Answers 2


Yes you should have ground conductors in the FFC to provide a return path for the signals. Connect the cable ground to the board ground which should also be your signal ground. This is reducing the loop, not making it worse. In this kind of configuration it is common to connect the ground plane of each board to a common metal chassis.

  • \$\begingroup\$ Please correct me if I'm wrong. If the FFC doesn't carry gnd signal there is no ground loop. (please show me if you see one) if you add the gnd you create the loop here I show the loop in big red loop \$\endgroup\$
    – pazel1374
    Apr 6, 2018 at 19:58
  • \$\begingroup\$ What is your concern about having that loop? \$\endgroup\$
    – EE_socal
    Apr 6, 2018 at 20:46
  • \$\begingroup\$ it create a big antenna that inject noise into my holy ground. the PCB #1 contain rf components (12-24GHz) which I dont want to degrade it performance with such a low quality grounding system \$\endgroup\$
    – pazel1374
    Apr 6, 2018 at 21:05
  • \$\begingroup\$ but before that you refer to a loop in your answer. where do you see loop in the design? \$\endgroup\$
    – pazel1374
    Apr 6, 2018 at 21:08
  • \$\begingroup\$ I am referring to the loop in your diagram, but I am not sure it is a problem. So you have two rectangular ground planes connected by one ground wire or multiple ground wires, its hard to say which is more of an antenna. The FFC with no grounds can also be an antenna. There are many other things that affect noise to be worried about such as proper PDN design and filtering. You did not mention how the boards are to be mounted. \$\endgroup\$
    – EE_socal
    Apr 6, 2018 at 22:59

High frequency return currents follow the path of least impedance. When your SDIO lines toggle, they cause a spike of high frequency current to flow as they charge up the gate of whatever is receiving them. A corresponding return current must appear (since you just charged a capacitor) and it will take the path of least inductance back to the driver. The edge rate of a 50MHz SDIO interface means that you have harmonics in the >1GHz range. These are not low frequency signals going over your SDIO cable. If you only have ground connections way over where you have them on your diagram, you just made a gigantic loop and you will cause your digital lines to have (possibly significant) inductive ringing since the inductance of the entire signal path (which includes the signal going to the receiver and the corresponding return current coming back to the sender) will now have a large inductance. To make matters worse, that large loop will now be carrying those >1GHz harmonics and instead of avoiding the creation of an antenna that picks up stray signals, you just made a radiator (signal comes out over FFC, return comes back over distant power cable: Loop).

A good rule of thumb for digital design is to have one ground line for every digital signal line (or use differential signaling) and then place each ground next to a single signal wire (1 ground per signal) to minimize the overall loop area.

As for ground currents, what it comes down to is a question of frequency. What return currents will flow over your power cable? The low frequency and DC ones (so long as you keep the DC series resistance smaller than the grounds in your cable, which shouldn't be hard since you should be using thick gauge wire). Which return currents will flow over the FFC cable? The high frequency ones that correspond to the switching of your SDIO lines. You want to provide ground paths for all the frequencies on your board, otherwise you'll surely make loops.

You can mitigate your concern in a couple other ways:

  • Shield your high-sensitivity RF circuitry separately. Very high frequency RF circuits sometimes go as far as to have a milled aluminum block that seats down on the PCB around the sensitive parts.
  • Use a big metal box and ground everything to it. Have your wifi antenna sticking out using one of those panel-mount RF connectors.
  • Move the power cable physically near the data cable. Have you looked at the pinout of PCI Express? The power and data are separated by possibly several inches, depending on the length of the PCB. But, there are consistent ground traces all the way across. I also suggest looking at the recommended grounding scheme of CompactPCI Express if you have access to that spec, as it will give you some hints on how industrial systems with strict immunity and emissions requirements deal with this multiple grounds issue.

Your Answer

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

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