# Voltage regulator output signal becomes noisy when connected to a CPU

I am currently working on a PCB where it has two onboard voltage regulators. the first one makes V1in=20 V to V1out= 5.5 V. The second voltage regulator makes V2in=5.5 V to V2out=3.3 V.

The 3.3 V voltage regulator used is 171033801 from Würth Elektronik. The output from the 5.5 V voltage regulator is stable regardless of the load on the 3.3 V voltage regulator.

The observations:

1. When no load is connected, the voltage regulator produces a stable 3.3 V output as observed in the first oscilloscope image.
2. When the CPU is connected to the PCB, the 3.3 V output becomes really noisy as seen in the second image.
3. There is a previous iteration of the board where another voltage regulator was used. The above issue doesn't present itself there.
4. The data sheet stated that it can provide up to 3 A output signal. When connecting the voltage regulator output to an electronic load, while increasing the load slowly, we could get only 0.7 A output load current until the voltage regulator shut off.
5. When switching the electronic load ON-OFF-ON, the load generates peaks in the current. The voltage regulator can only supply 0.5 A without turning off.
6. We tried giving up to 34 V as input voltage so as to see if we can get the total 3 A current. We could only measure 1 A at the output.

It's difficult to tell in this image, but on the top are the input capacitors, three of them (47 µF, 2 x 4.7 µF), followed by a 1 µF cap, and the voltage divider resistor that sets the output voltage. To the right is the 5.6 kΩ resistor which sets the switching frequency and to the bottom is the 47 µF output capacitor. I am also adding the 3D model to make it a little easier to understand.

I have also tested the PCB with three more voltage regulators since then, two from eval boards from Würth Electronic (178021501), this has Vin = 10 V but produces 3.3 V) and the 178023801. This has the same voltage regulator type but produces 2 A instead of the 3 A that is on the board.

I have also tried using the L5973D on a separate PCB, and in all three cases I have connected the output to the output cap of the voltage regulator (voltage regulator removed) and they work with no noise on either of the voltage lines(5.5 V and 3.3 V) and the CPU starts up.

I have some new voltage regulator, the same kind that is present on the PCB, I will replace these regulators and see if that helps.

I am beginning to think this maybe a faulty regulator, but that just seems like a easy explanation and im not satisfied with it. The reason for this is because I have 30 PCBs which produce different results when hooked up to a power supply. Some do not produce any output i.e., output is 0 V, some produce a sawtooth-like waveform at about 600-900 mV, and the others produces the above type of noise when the CPU is connected.

This makes no sense since if this was a routing issue, it should not work with the other voltage regulators. I would need a second opinion before I write this off as a faulty regulator.

Edit: I havent come around to doing the testss with regards to what @Deam Franks mentioned, but it seems close to what i think might be happening. I spoke to a person from Würth Elektronik, and he said that there might be some paraitic impedance or transient effect due to the ground planes on the input caps being a seperated and connected only through a via. He also inclined towards maybe a input filtering problem. This makes sense but it doesnt really explain why it works upto 0.5A - 0.7A and stops working after. When i connect a USB to supply the PCB, it introduces alot of noise on the output 3v3 and the input 5v voltage rails. Sometimes I also get 0.85V which is approximately the same as when no feedback from the volatge divider. He said there might be also be a problem by having cold solder points, or something might have gone wrong in the manufacturing process but cannot be sure. He will come next week and give it a once over.

Edit:

The field Application Engineer from Würth Electronik had come around and checked the PCB and ran a few tests. He said that the voltage regulator needs a clean ground plane for the return path. Here in my design i have a trace cutting through this plane at the input capacitors and this is the cause of the volate regulator not working. The Regulators keeps switching between soft restart phase. We did a few tests by adding a cap across the voltage regulator and connecting the grounds together externally with small wires. This seemed to improve the working of the voltage regulator, as we could get about 0.5A more output current as when without. In all the board would need a redesign and better grounding at the voltage regulator and this should fix the issue.

• Try brute force filtering, e.g., 0.47 µF ceramic and 470 µF electrolytic capacitors in parallel with the existing 47 µF cap, and, if that is insufficient, add a series inductor before the caps. Commented Mar 25 at 15:50
• What filter caps are installed on the supply pin of the CPU? Commented Mar 25 at 19:55
• If you are measuring the supply at the CPU itself, and seeing those dips, then you should put extra ceramic bypass caps right there, at the CPU. If this is being measured close to the regulator output, and bypass caps there don't help, then the regulator itself is rubbish. A clue is that it's happening every 25ms, which makes me suspect insufficient bypassing at the CPU itself, and across whatever load is being switched at 25ms intervals. Commented Mar 27 at 16:27
• What does the input to that regulator look like in the high noise state and when it shuts off? If your noise occurs at very light loads, it could be because of cycle skipping at light load. Commented Mar 27 at 19:40
• If you see similar noise at the input, put a resistor in series (before the input caps on the second regulator) and see if there is more noise on the source or sink end of the resistor (or the same). At 0.45A you should not be in pulse skipping. If you put in a series resistor, put one on the output too and probe (differentially) across the resistors to measure the current waveform with the noise waveform. If they are synchronous, you have a transient response / filtering issue. If they are mostly uncorrelated you might have a switching or input filtering problem. Commented Mar 28 at 18:25

Assuming 4 layers with continuous ground plane on layer 2.

1. Should use direct connect instead of thermal relief connect for the copper pour. The thin traces created by thermal relief add inductance to the input caps.

2. Needs more than 1 ground via, ideally 1-2 per cap.

3. I don't see any vias connecting the GND pad of the switching converter to the ground plane. There's probably one somewhere, otherwise the design rule check would complain, but you'd need a bunch of them around the ground pad.

1,2,3: This adds inductance both in the hot loop (input caps-switches) and to the C207 which decouples the chip's internal VCC.

1. Due to high inductance between the GND pad and GND plane, the whole ground copper pour is going to get a lot of noise when the internal lower MOSFET switches. It is directly connected to the ground leg of the feedback divider, so it will pump noise into the feedback voltage.

I think the culprit is either 4, as it makes the chip think the output voltage is higher than it is, so it will think overvoltage is occurring and back off, as the scope shows. Or 3, as the internal VCC will drop when the MOSFET drivers need some current, which can reboot the chip.

The feedback resistor should have its own via to the ground plane, and not share a copper pour with anything else.

• I am marking this as the answer as this was closest to the issues I encountered on the board, and also similar to the reply I got from the fields engineer from Würth Elektronik. Also the tips on the routing will be used in the new redesign of the board as Its difficult to test the rest of the board without a working 3v3 voltage regulator. Commented May 16 at 5:18
• Thanks and have a nice day! Commented May 16 at 5:41

on page 20 of the datasheet they show some typical transient response of the regulator, which is not that different from your measurements.

The quoted 3A current is a maximum DC out and hasn't got much to do with the pulses you see as the load varies sharply.

The best way to deal with this is decoupling, decoupling and more decoupling, especially large caps placed near to the point where the sudden load change occurs. The point of those caps is to supply short term current demand, so the regulator is essentially just used to "replenish the tank". If your load impedance changes sharply and causes sharp changes in load current, large decoupling caps, selected for low ESR are your first and best remedy. Even if you could fix this by choosing a regulator with better transient response, it's not ideal as those current pulses create noise which radiates and makes your life harder in other ways.

Decoupling is king, and in general there is no such thing as too much. (Well there is, but it is a far better problem to have.)