1
\$\begingroup\$

I am currently designing a PCB for a PWM controller based on the LMC555 timer chip along with a low side gate driver FAN3100TSX and N channel power MOSFET. Below is the PCB in question. In my design, I have separate ground planes, one on the left side is for low power analog section and on the right side is high current analog section. I have created a common connection for ground planes at the top middle (at pin 1 of J1 ). Essentially this would be my star ground connection. Additionally, the gate driver FAN3100TSX (IC2 on board) requires pin 2 to be common ground for chip for both control signals and power signals. Because I'm using the driver in non-inverting mode, its IN- pin (pin 4) needs to be grounded. This IN- counts as control signal pin. Thus I have made a connection between pin 2 and pin 4 to create common signal ground for the IC. I have also connected pin 2 to the high current ground plane on right because of return currents when it drives the Power MOSFET. So my question is, does this connection between these two pins create a ground loop and cause problems? Is there a different way to do this and create a star ground? Any suggestions. Thank you

This is whole PCB: enter image description here

Zoomed in at J1:

Zoomed in at top of board

Zoomed in at IC2:

Zoomed in at bottom of board

\$\endgroup\$

1 Answer 1

1
\$\begingroup\$

The question that needs to be asked is: "Do I need separate planes?"

The answer is usually "No"

Here is why:

By separating the grounds, there is only a small piece of copper in between the two planes. This copper has inductance and resistance, so what is done in this design is like putting a small inductor and resistor between the two planes.

The resistor made from the trace will be about 1mΩ with maybe 1nH of inductance, which will make a filter on the ground for the left half of the board. Any current moving from the left hand side of the board will flow through this point and create a small voltage through the resistor/inductor trace.

enter image description here

The biggest problem will be IC2 (blue) which the signals connected to it are referenced to the right half of the board and it's ground is referenced to the left half of the board so any difference in voltages on the grounds, which could be in the mV's depending on the current.

Another problem is the entire ground plane forms a nice dipole antenna, which could also create EMI problems or ring at high frequencies.

So unless there is a good reason, don't split the planes and combine them and let everything be the same potential. The best way to deal with return currents is with board layouts that rout the currents to the right paths (currents take the path of least impedance (resistance) or the orange lines. And it looks like the current's won't cross anything important (if they do a chip that is ground referenced might see the currents, V=IR and ground planes have resistance).

If you want to eliminate a ground loop (like if the connectors are connected to other devices) then isolation is the best (like optocouplers or digital isolators)

\$\endgroup\$
3
  • \$\begingroup\$ I guess my intent was really to create a star ground thinking it was best for the board and keeping the high current away from input side of IC2. I did intentionally keep components for IC2 together and high current components near to right. I hope this is enough. So it’s ok to use a full ground plane across whole board and it won’t cause any issues? \$\endgroup\$
    – Leoman12
    Commented Jan 27, 2021 at 5:35
  • 1
    \$\begingroup\$ What I am saying is that it will create more issues then it saves. The high current will travel back to the ground pin and away from the other components (it spreads out but mostly follows the shortest path back to the ground pin). It is ok to use a full ground plane \$\endgroup\$
    – Voltage Spike
    Commented Jan 27, 2021 at 6:48
  • \$\begingroup\$ Ok, that does make sense. Thank you. \$\endgroup\$
    – Leoman12
    Commented Jan 27, 2021 at 13:13

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.