Reducing ripple voltage in 2 MCU circuit

[doru.cazan]

Hi All,
I have a board using 2 MCUs: one lower power (less than 20mA), continuously running and one higher power (more than 500mA) that runs from time to time. The main power is 24V ac with a step down buck converter that can deliver 1.5A at 3.3V. It works fine (ripple below 40mV) when the higher power MCU is not running. However, when the higher power MCU starts, due to its power consumption that varies a lot (wifi camera stream), the ripple voltage raise to about 200mV. The top diagram in the attached image is the simplified current design.
Would raising the step down output voltage to 3.9V and adding separate LDOs for each MCU help keeping the ripple voltage low enough  ? The diagram for this scenario is the one at the bottom of the attached image.



Many thanks!

[tszaboo]

The issue is likely with your selection of DC-DC stepdown and the power delivery network. This means capacitors, planes, tracks. 500mA is not a lot. The only time you would need separate power supplies for this is in case you are running very sensitive analog parts on your first MCU.
I would add a 100uF or so electrolytic capacitor as a start. You should also post your layout, and stackup.

[doru.cazan]

Thanks @tszaboo,
Here are the details of the buck converter (attached images). There is a 4 layers board and tried to design the PCB as close as possible to the data-sheet recommendation. The components values are the ones from WEBENCH® POWER DESIGNER with the difference that I doubled the input and output ceramic capacitors (10uF and 100uF)-orange rectangle. The low power MCU is an AVR, it will run at 10Mhz and there are 10uF, 1uF and 0.1uF capacitors very near it so probably it is fine; the second MCU is and esp32-s3 and about 200mV ripple is, I think, dangerously close to the 3V lowest power requirement for it... if possible I would like to reduce the ripple and I do not mind adding the LDOs if those will help: it is a hobby project so the cost for one board is not relevant in this case. it is just that I am not sure if adding LDOs it will really help reducing the ripple...
I can also test it with an electrolytic cap but there are already 2 x 100uF ceramic caps in parallel for the 3.3V output voltage and the enclosure will be really thin; not sure how many uF I can squeeze inside (height from the PCB to the enclosure is about 7mm)  Oh! I would like to avoid tantalum caps if possible.

[selcuk]

The inductances of 3.3V and GND nets may cause an issue. You can short F1 to see its effect. Additionally you can use a star connection for GND net going to the MCUs. Is 3.3V net going through a single via?

[mariush]

If your input in 24v AC , that gets rectified to Vdc peak = sqrt(2) x 1.414 - 2 x forward voltage of diode  = ~ 32v  ... HOWEVER, idle voltage of a transformer is often 10-15% higher, your mains AC is often higher (for example 245v AC at 2-3am instead of 230v AC) so your peak DC voltage can be more than 35v.

When only your microcontroller that consumes 20mA is active, it's as if the transformer is under no load, so its output may be much higher.

Your LMR33630 is dangerously close to that peak voltage, it has a maximum input voltage of 36v.  Maybe you could add some protection in the form of a zener diode that engages at ~33v but you'd be better off with another regulator.  Example zener diodes 33v : https://www.digikey.com/short/hn0v5h02


Anyway, you need around 550-600mA on 3.3v - that's 2000mW, assuming around 90% efficiency, you need around 2200mW on input ... that's around 100mA at 22v .. let's say you want at least 24v at 0.1A load.

Capacitance in Farads = Current / ( 2 x AC Frequency x [ Vdc peak - Vdc min desired] ) ...  = 0.1A / ( 2 x 50 Hz x (32-24) ) = 0.1 / 800 = 0.000125 Farads or 125uF.

You could lay them horizontal or the board, or maybe consider having a cutout on the pcb to add the capacitors...

example

6.3mm diameter 47uF 50v rubycon :  https://www.lcsc.com/product-detail/Aluminum-Electrolytic-Capacitors-Leaded_Rubycon-50YXJ47M6-3X11_C88791.html

8mm diameter 100uF 50v rubycon (if you make cutout in pcb it would fit in your case) : https://www.lcsc.com/product-detail/Aluminum-Electrolytic-Capacitors-Leaded_Rubycon-50YXF100MEFC8X11-5_C88728.html


You can get polymer capacitors for higher current rating... ex

6.3mm

47uF 50v 6.3mm diameter, 8mm tall  : https://www.lcsc.com/product-detail/Solid-Capacitors_AISHI-Aihua-Group-SPZ1HM470E08O00RAXXX_C122243.html

8mm

220uF 50v 8mm diam : https://www.lcsc.com/product-detail/Solid-Capacitors_NJCON-2210500816R00_C5373403.html

100uF 50v 8mm diam : https://www.lcsc.com/product-detail/Solid-Capacitors_AISHI-Aihua-Group-SPZ1HM101F09O00RAXXX_C171434.html

If you can guarantee voltage won't get close to 35v, you can get better capacitors

ex 220uF 35v 6.3mm diameter : https://www.lcsc.com/product-detail/Solid-Capacitors_AISHI-Aihua-Group-SPZ1VM221E12O00RAXXX_C171433.html


As for the regulator IC, something like AP64060 would seem ideal for you : https://www.digikey.com/en/products/detail/diodes-incorporated/AP64060WU-7/16399099  or (automotive qualified) https://www.digikey.com/en/products/detail/diodes-incorporated/AP64060QWU-7/16186480

It's max 40v in, outputs up to 600mA, works at 2mhz but also has a fpm mode to be more efficient at low loads 

LMR51606 is another option, available in either 400kHz (X) or 1 Mhz versions (Y) , goes up to 65v in, up to 600mA output, and for each you also have the fpm only version (more efficient at low loads but higher ripple) or fpwm (force pwm, lower ripple but less efficient at low loads)


fpm 400 https://www.digikey.com/en/products/detail/texas-instruments/LMR51606XDBVR/22116882

fpwm 400 https://www.digikey.com/en/products/detail/texas-instruments/LMR51606XFDBVR/22116849

fpm 1.1m https://www.digikey.com/en/products/detail/texas-instruments/LMR51606YDBVR/22116848

fpwm 1.1m https://www.digikey.com/en/products/detail/texas-instruments/LMR51606YFDBVR/22116862


EDIT:  I read  UP TO 500mA,  but I see now that it's MORE THAN 500mA.

In this case the above regulators won't do, but there's others that can do more current

AP64102 / AP64102Q is good for 1A : https://www.digikey.com/en/products/detail/diodes-incorporated/AP64102SP-13/17050624

AP64202 / AP64202Q is good for 2A : https://www.digikey.com/en/products/detail/diodes-incorporated/AP64202SP-13/14123506

AP64352 / AP64352Q goes to 3.5A of current : https://www.digikey.com/en/products/detail/diodes-incorporated/AP64352SP-13/10420692

All go up to 40v in, and default to 500kHz but can be configured at lower frequencies using a resistor, between 100kHz and 2.2 Mhz.

LMR36520 can do 2A and supports up to 65v input

[doru.cazan]

Thank you @selcuk, @mariush

The inductances of 3.3V and GND nets may cause an issue. You can short F1 to see its effect.

Tested. Ripple voltage went down from ~200mV to mostly 60mV, rarely 100mV. @selcuk, would it help to place the fuse further away?

Is 3.3V net going through a single via?

Yes. Unfortunately for me, I have no idea (=knowledge) to understand if this is helping or not 

If your input in 24v AC , that gets rectified to Vdc peak = sqrt(2) x 1.414 - 2 x forward voltage of diode  = ~ 32v  ... HOWEVER, idle voltage of a transformer is often 10-15% higher, your mains AC is often higher (for example 245v AC at 2-3am instead of 230v AC) so your peak DC voltage can be more than 35v.

Maybe you could add some protection in the form of a zener diode that engages at ~33v

@mariush: based on "- 2 x forward voltage of diode", I think one more diode in series plus a zener diode? Just need to find a diode with a forward voltage that is not really low... I am thinking of this "solution" because will keep the changes to a minimum.

Your LMR33630 is dangerously close to that peak voltage
..AP64102 / AP64102Q
..AP64202 / AP64202Q
..AP64352 / AP64352Q
..LMR36520

Will think about testing other regulators. Have a similar device running for 5 years with MP1584, max 28V in the data-sheet (not the best!), tested AP64350 and LMR14030S before. The biggest pain point here is the temperature raise. All (MP1584, AP64350, LMR14030S) raised from 24°C to near 40°C with minor variations. LMR33630 is the first regulator I tested that raises from 24°C to no more than 32°C. Considering the enclosure is very small, this is one of the main design points.  LMR36520 looks like a good option since it is pin compatible but I am worried that the RDS-ON values in the data-sheet are almost 3 times higher than for LMR33630; instead of a temperature raise I prefer to add more diodes in series 

Capacitance in Farads ... 6.3mm diameter 47uF 50v rubycon

I already have 3 x PANASONIC EEEFT1H470AP (3 x 47uF 50V) on input, also the 2 x 10uF ceramic capacitors:

Will de-solder one and replace it with a larger capacitance to test if behaviour improves.

Many thanks!

[radiolistener]

Would raising the step down output voltage to 3.9V and adding separate LDOs for each MCU help keeping the ripple voltage low enough  ? The diagram for this scenario is the one at the bottom of the attached image.

yes, it also require low pass filter with ferrite beads before regulator and ceramic+tantal capacitors on MCU power to reduce noise level and reduce noise leakage from MCU to a power bus. Also proper PCB layout is required

Regarding to PCB layout, the input capacitor, output capacitor, and the inductor should be placed as close as possible to the IC in order to reduce RF interference and ripple. In your case it's a little bit too far, it may cause some issues

[mariush]

You don't have a temperature problem ... 40c is not really that hot.

You can reduce the temperature through other means, like better placement of the regulator IC - if you place it more towards the center of the board, the center pad will transfer heat and the heat will radiate in all directions of the circuit board over a larger area, so the chip will potentially be cooler.  In your layout, you have the IC in that bottom right corner, so the heat can only go in two directions.

You can also get better heat transfer with thicker copper, ex 2oz copper on top would be better than 1oz or less.

I don't see 3 electrolytic panasonic capacitors in your schematic and pictures of the board.

Those electrolytic capacitors you chose aren't great. Surface mount electrolytics in general aren't great. Your 47uF 50v capacitors have a ripple current of 195mA and 0.68 ohm ESR (not that important for "buffering" output of a bridge rectifier).

The Rubycon ones I linked to (47uF 50v) are rated for 295mA current and the ESR is half at around 0.3 ohm. They're also rated for 7000h at 105c compared to Panasonic's 2000h @ 105c

The polymer ones I linked to are 6.3mm x 8mm and have current rating of 2.1A and ESR in the 30-40mOhm range. They're rated for 2000h@105c but it's different rating compared to electrolytics, it's more like over 30k hours of electrolytic equivalent.

With electrolytic capacitors you can approximate double the lifetime for every 10c decrease in temperature, so for example at 45c ambient temperature a 7000h @ 105c would be 14k at 95, 32k at 85, 64k@75, 128k at 65m, 256k@55, 512k@45c

With polymers it's more like lifetime = original lifetime x 10^{(rating - ambient)/20}  so for example at 45c internal temperature, you'd get 2000h * 10^(105-45)/20 = 2000h * 10³ = 2000*1000 = 2,000,000 hours 

They also take much less space compared to your surface mount capacitors if layed flat on the board, you could have two of them with the leads on the center of the board like this

[=] C1
[=]
+ -
+ -
[=]
[=] C2

Don't even need holes if you don't want the back of the circuit board to be broken, you could solder the leads to pads and lock the capacitors in place with a bit of glue or threadlocker liquid.

The surface mount bridge rectifier you chose seems to be rated for 1A or some lower value, you may want to see how how the current goes, as you say you'll need more than 500mA on the output


Yes, you need 3.3v trace and everything to be thicker/wider, going through a via is bad idea.

The sizes of the input capacitors seem a bit off..  I would expect that 1uF ceramic to be 0603 X7R and the 10uF to be 1206 or 1210 and rated for at least 75v, 100v would be preferred....  maybe something like this : https://www.lcsc.com/product-detail/Multilayer-Ceramic-Capacitors-MLCC-SMD-SMT_Murata-Electronics-GRM32EC72A106KE05L_C576517.html

Your design is also kind of weird because you have the AC input of your rectifier towards the middle ... you're running AC voltage close to 3.3v output (may be on separate layers or with enough distance but still odd ... think about if there's some water getting inside the device, is your ac separate enough from output?


The forward voltage of a diode varies with the current ... a diode may drop 0.8v at 1A but may drop only 0.4v at 50mA ... your problem is at low loads, when your high consumption device is turned off... the transformer's output will be higher, even higher if your mains voltage is high, and the bridge rectifier will drop less voltage so they all add up and you end up with high voltage. Adding one or two diodes won't do much because they'll also drop little voltage due to low current.

See for example https://www.comchiptech.com/admin/files/product/DF2005S-G%20Thru340691.%20DF210S-G%20RevF.pdf  - look at Figure 4 on page 2, you have nearly 0.6v at <100mA, and up to 1v at 1A. This forward voltage also changes with temperature but that's less important.

If you do use a zener diode, you'd probably want to add a resistor after the capacitors to limit the current going through the zener diode when you have those excess voltages otherwise the diode could be damaged. Don't know what value, something small

[selcuk]

Tested. Ripple voltage went down from ~200mV to mostly 60mV, rarely 100mV. @selcuk, would it help to place the fuse further away?
Yes. Unfortunately for me, I have no idea (=knowledge) to understand if this is helping or not 

Yes. Adding additional vias to 3.3V net may help. This leads to a reduced inductance since you are paralleling via inductances. Seems that fuse impedance is high enough to disturb the operation. It is the same impedance if you move it away. I don't expect an improvement.

Pleaase read "12.1.1 Conductive Coupling" chapter and Fig 12.3 of this book. The common impedances of two circuits causes the noise to propagate from one to the other.
https://link.springer.com/chapter/10.1007/978-3-031-14186-7_12

[tszaboo]

Thank you @selcuk, @mariush

The inductances of 3.3V and GND nets may cause an issue. You can short F1 to see its effect.

Tested. Ripple voltage went down from ~200mV to mostly 60mV, rarely 100mV. @selcuk, would it help to place the fuse further away?

I'm not sure why you would have a fuse on the output of the converter. Fuses are used on PCBs for one purpose. You have a minor fault, like a short circuit, and you want it to avoid turning into a catastrophic fault, like a fire. On the output of the converter, it's not going to fulfill that purpose. You should move the fuse to the input of your circuit, before any active parts.
More vias can help, they are free. Or bigger via.
What's the purpose of D4? Do you have a crowbar on the output of the buck converter?
I have some experience with these ESP modules, they like to have a large electrolytic capacitor on their power rail. From what I can see stability related issues can be traced back to the lack of these in the circuit.
Your DC-DC converter layout is OK. You could improve it with more vias to ground, and smaller loop areas, but I've seen much worse. You should add testpoints to your circuit though.

[doru.cazan]

Many thanks to everyone helping!!! So many good ideas!
Listing my take-away learnings so far:

I'm not sure why you would have a fuse on the output of the converter...
What's the purpose of D4? Do you have a crowbar on the output of the buck converter?

It is the same impedance if you move it away. I don't expect an improvement.

Yes, I was thinking to use a crowbar for protection. Will move the crowbar before the buck converter.

Yes. Adding additional vias to 3.3V net may help.

More vias can help...Or bigger via.

will definitely do!

Your LMR33630 is dangerously close to that peak voltage, it has a maximum input voltage of 36v.

Very good point. There are:

• LMR36520 pin compatible but higher RDS-ON values
• LMR36015 or LMR34215
• AP64202 looks like a good alternative (new design required)
• AP64352 looks like the best alternative; similar with AP64350 tested before

I think next should test both LMR36520 and AP64352 (for AP64352 re-design the PCB) and see how low I can keep the temperature.
Will it help (lower ripple, lower temperature) to use the automotive-compliant AP64352Q?

Those electrolytic capacitors you chose aren't great.
They also take much less space compared to your surface mount capacitors if layed flat on the board, you could have two of them with the leads on the center of the board like this

[=] C1
[=]
+ -
+ -
[=]
[=] C2

Will definitely look at alternatives for capacitors: 220uF 50v NJCON looks good and I can use one instead of 3 but will require a cutout in the PCB. Anyhow will run a seach for leaded solid capacitors before making any decision.

You can reduce the temperature through other means, like better placement of the regulator IC.

Yes, will look how I can improve the design of the PCB to keep the temperature as low as possible!

You should add testpoints to your circuit though.

Good idea, will do!

Pleaase read "12.1.1 Conductive Coupling" chapter and Fig 12.3 of this book. The common impedances of two circuits causes the noise to propagate from one to the other.
https://link.springer.com/chapter/10.1007/978-3-031-14186-7_12

Thanks, much appreciate for sharing it!