I'm designing a power source for one of my projects and I couldn't find a better way to reduce the voltage drop on 7805 regulator other than using a switching regulator (LM2596).

The switching regulator output goes through an additional LC filter (with tantalum caps) and from there to a linear regulator:

The filters and linear regulator should filter out most of the switching noise, my only concern is that the noise can spread through the PCB traces, here's the one sided PCB design (those front coppers are actually jumpers):

LM2596 current is not going to exceed ~200mA.

I don't have any experience in designing switching regulators and handling noise, all I did was "pouring" the ground line.

  • How can I reduce the output noise (as much as possible but reasonable) in this specific design?

  • How to prevent the inductive noise in PCB design?

  • 1
    \$\begingroup\$ design critique: why only go down to 12 V if you want 5 V in the end? Try 6V and a modern low-dropout (LDO) 5V regulator instead of the antique LM7805; modern linear regulators have better transistors and faster control loops, drastically improving noise reduction. But: when designing something, always state what you need to achieve before even starting to design. So, what amount of switching noise in which frequency bands do you care to achieve? \$\endgroup\$ Jun 6, 2020 at 17:49
  • 1
    \$\begingroup\$ @MarcusMüller The switching regulator output is 7V not 12V! that 12V AC is another secondary of the transformer. I didn't use LDO regulator because older ones are cheaper, LF50 was one my options though... about the noise; ideally what I want at the output is dead linear but even if I was willing to go that far, I don't have the equipment to scope the output. so I'm trying my best to reduce the noise as much as possible... please point out any other error in the PCB if you spot any, I'd appreciate it. \$\endgroup\$ Jun 6, 2020 at 18:10
  • 1
    \$\begingroup\$ yeah, no, "as much as possible" would dictate you build this circuit out of superconducting stuff cooled down to close to absolute zero. Which is quite the opposite of "I tried to save a few cents on linear regulators". Also, you really don't need "as little noise as possible", you need "as little noise as my application can accept", and you've not told us what this supply is for! \$\endgroup\$ Jun 6, 2020 at 18:17
  • 1
    \$\begingroup\$ hm, if you're building a low noise reference, shaving cost off the supply doesn't sound the right thing to do for now. \$\endgroup\$ Jun 6, 2020 at 18:32
  • 1
    \$\begingroup\$ Why make your linear supply worse by replacing it by a zener? Don't! use a modern linear regulator, follow the low-noise supply application notes written by the regulator manufacturers :) \$\endgroup\$ Jun 6, 2020 at 18:52

1 Answer 1


For lowest noise, you need GND of C4 next to GND of D7, TO MINIMIZE that loop_size/radiation/voltage drop. Why? The slewing of the diode voltage (input to energy storage inductor) will be the fastest node in your system. Keep that PCB trace very small in area and very short in length (which also reduces the radiative loop area); and have a trash collector (piece of copper, tied to Gnd) under that very fast 24 volt switching-reg node.

For less "singing" at the 60 Hz rates (or 120 Hz rate) from very fast current_turn_on thru the bridge rectifier, insert 1 uH inductors or 1ohm resistors in series with 1 leg of the bridge.


Does everything look fine? What are your noise goals? (for lowest noise, use a 2nd layer as GND plane.)

Is this to evolve into a commercial project, with formal must_pass_FCC measures? Is so, why not START by using a GND plane?

Have you considered how to remove heat? A 1_layer PCB will be horrid at heat removal because the epoxy_fiberglass will define the heat flows; FR-4 has 200X the thermal resistance of copper for equal thickness; the ratio of thicknesses is about 0.060 / 1.4 === 40X, so the heat flows will be very limited; expect local HOT SPOTS.

To understand this, get a quadrille paper pad, and start drawing heat sources and heat exits, realizing each square on the pad is an increase in temperature.


The 60Hz (120 Hz) singing is the narrow/fast turnon time of the DIODES in the bridge (4 diode) rectifier. Assuming most of the turnon current occurs in 0.026 volts (when the current thru a diode increases by e^1 = 2.718^1 = 2.718X), your turn_on time will be the SlewRate of your unrectified power transformer output, divided into 0.026 volts.

Assuming SlewRate of transformer is 40 volts peak * 377 radians/second (from taking the derivative of 60Hz sin, with 6.28 * 60 == 377) or SlewRate is found to be about 16,000 volts/second. the turnon time is 0.026 / 16,000 == 1.5 microSeconds.

Thus your 60Hz rectifier diodes are a 1.5 microsecond fast-edge high-power interference generator.

  • \$\begingroup\$ 1. what do you mean by "trash collector"? 2. "insert 1UH inductors or 1ohm resistors in series with 1eg of the bridge." what's 1eg? it's a hobby project there's no goal, just to reduce the noise as much as possible. the heat generated by the switching regulator or linear regulators? for linear regulator I'm going to mount a heatsink and for switching regulator I'm going to take your advice and go with 2 layer PCB. that should be able to sink some of the heat as it is mentioned in the datasheet. \$\endgroup\$ Jun 6, 2020 at 16:11
  • \$\begingroup\$ That 60Hz singing you mentioned is caused by switching regulator inrush current? I did compensated for that by using ON/OFF pin of the regulator and C7, R3 and R4 as datasheet recommended and I increased the delay a little bit more. isn't that enough? \$\endgroup\$ Jun 6, 2020 at 18:34

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.