PCB design - noise and ground loop

Question

I'm working on a electronic load and it's not very sensitive to noise, the questions are mostly out of curiosity.

• On the PCB I have a fan control circuitry that I separated the ground and positive path and going to connect them separately with a twisted pair of wire directly to power supply. is doing this helps to prevent the fan noise to spread?

• There's a high current path on the PCB (marked with arrows) that I have to join its ground with analog ground, is two grounds connected together correctly (marked with circle)?

• I'm measuring voltage drop over a shunt (marked with square) with a diff-amp, is the differential path connected correctly?

• I'm a bit confused about ground loop, the ground plane goes around the PCB. meaning a single node can have two paths to ground. Do I need to cut the trace (marked with X) so that current flows only in one direction?

Answer 1

These aren't questions of right or wrong, as with a lot of PCB design, it's about how much effort/cost you want to expend, and how much devaition from perfect you can tolerate. That's PCB design in a nutshell.

Nothing in that layout immediately jumps out to me as wrong. Paths are short and direct, no huge loops, no tiny traces. If I look at the NE5532 I see and max BW of 140kHz, so I would think this board would be fine at those kind of frequencies, assuming the design is sound.

1. Twisting pairs together is more a technique to reduce noise coupling into a pair of wires, than it is to prevent noise travelling along the wire. I wouldn't recommend seperating the GND and power supply like that, as it can create EMC issues if not done well. The better option if you're really worried about noise from the fan would be to filter it. The more worried you are, the more complex the filter. You can start with some bulk decoupling, or add an LC like ElectronicsStudent suggests.

2. Probably, but it depends on how much current is passing, and how wide the gap is. A bigger, more solid, shorter ground connection is always better, but not always needed. Are we talking 1, 10 or 100A? Is this DC, or is there switching involved? Aproximate the path as a rectangle, then use a free calculator (google saturn PCB toolkit) to figure out it's DC resistance, usually that'll be enough to figure out if it's likely to be a problem or not.
3. Your schematic is incomplete, so it's still impossible to say if this is going to work. That being said, the feedback seems a bit odd to me. When/if the output of U2B goes low, D5 and D6 from a "sort of" clamp to Vout + 3.7 + 0.7, though in reality this will be more defined by leakage. D6 can just forward bias, leaving D5 to leak, or the other way around. If this is an electronically controlled load U2B is controling the MOSFET gate such that the current is controlled, then I'm not 100% sure this is how to do it. I might also consider adding a capacitor in parrallel with R25 to form a low pass filter.
   Your question is more about the routing than the schematic though, so comments aside, I can't see anything bad in the routing. At the frequencies you're using I wouldn't be worried.

4. Issues of ground loop apply more to large systems with longer cables. A classic is sound systems, were long cables to connect instruments to a mixer, particularly where there's power generation at both ends, a mis match in ground potential can cause currents to flow in the ground, which directly creates noise. Also, you can have issues where a signal takes one path (becuase there's only one connection) but it's return (because every signal must flow back along a ground (usually)) might flow a different way if there's multiple ground paths. In PCB design however, ground loops aren't really an issue. If you had multiple layers, you'd actively take steps to connect them together at multiple points. Is is important at higher frequencies to consider the return path for a signal, and ensure there is an unbroken path that matches the signal path, but not really at this frequency. For a 140kHz board, just make sure there is a GND path. Don't cut it anywhere.

Answer 2

(1) If your fan is PWM controlled, I'd consider adding a L-C filter in the V+ path towards to PWM controller. Give it nice bulk capacitance and an effective suppression value at the nominal PWM frequency.

If it is an voltage controlled DC-fan, some capacitance at the controller V+ will solve all problems.

(2) I personally never separate grounds! There are more issues with it, than problems solved. On a single-layer PCB this is different - but I have little experience with that.

(3) Can not tell without schematics.

(4) Ground-path is a bit misleading. If your are talking 'pure physical DC' then it's an question of DC-resistance. But, real circuits are never 'true DC'. Therefore, depending on your frequency components the current will take different paths. The energy will not even flow through copper at all in some cases. It's weird.

I would not cut the trace - There is in my opinion no good reason to intentionally worsen your ground connection.