First attempt at an SMD PCB - breadboard power supply

[ilium007]

First attempt at an SMD PCB design below. I decided to build a breadboard power supply (yes I know I could buy one from AliExpress for $1.29) to learn KiCAD and PCB design techniques.

I have 2 x AP2112K-3.3 LDO voltage regulators and have a question about the output capacitor connections. Can I just connect them as shown in the left regulator below with 30mil tracks or should I use a copper pour as in the right hand regulator? Should I have it solid connected to the SMD pads or should I be using thermal reliefs? The via's are there only to experiment with them.







Should I use 30mil tracks for the output capacitors:


or should I use a copper pour:

[bateau020]

My suggestions:
* thermal relief is not really needed if you hand solder, not on this type of circuit.
* you could make it single sided, will give you even more freedom for manufacturing. If you want to experiment with the enable pin, why not route them to a 2 pin header with jumpers?
* input power protection (reverse, overvoltage) is lacking. A TVS or maybe even an ideal diode may be nice.
* input filtering could be better: add a 100nF on the input. You might even try adding a choke or a common mode choke.
* no real need for the 10uF on the output. That chip is stable at 1uF, and adding too much might may even hurt you, depending on the load. There are some topics on this forum about that subject. But it is very probably OK as is. Just add caps on the right places on your breadboard.
* this board WILL suffer from shorts and overloads. I suggest using the SOT89-5 version of the regulators, not SOT25. About 2 times better heat dissipation. Add a lot of copper around the tab for heat dissipation. And get real ones, not from ali or ebay. As designed now, you will probably smoke them very quickly.
* you should probably make the 5V and 3V3 lines wider, and get the LDOs closer to the headers.

But all in all, this is for breadboard, and the power distribution quality will be low anyway, so no real need to overdo it.

[ilium007]

Thanks for the reply. I need to find more information on the input / output capacitors. The 10uF is used on all the Adafruit boards using this LDO regulator so I thought it would be a safe bet! I'll try and find the forum posts in the topic. I left reverse polarity protection off because I figured it would be unlikely to achieve given the USB sourced voltage input to the regulator.

[ilium007]

I've found what looks like a better LDO regulator....

LDL1117  https://octopart.com/ldl1117s33r-stmicroelectronics-81876163?r=sp

Much lower dropout voltage of 350mV at 1.2A. I am still confused by these input and output capacitors. The datasheet shows 'typical' input / output capacitor values and it says that I can use ceramic capacitors. Do I just go with the 1uF / 4.7uF values? Surely I have to consider the transient loads involved? This breadboard is just a test circuit for a 3.3v supply I will use for an ESP32 based project.



The stability graphs seem to indicate that for very low ESR (assume thats what my MLCC will be given there are no ESR specs documented in their datasheets) a 22uF is best.

[ilium007]

And why doesn't [ Attachment Invalid Or Does Not Exist ] work on this forum??!!

[JustMeHere]

Yes, you will need to account for load transients.   I know from the hard way a ESP8166 or an ESP32 need at least 200uF of bulk capacitance.  I put these next to the VCC pin of the chip that needs the power.  I still keep the small output cap near the voltage regulator though.

Is this correct?  Well it works. Dave showed in a video that bulk cap placement isn't super important.

[bateau020]

Capacitor values depend in the regulator you use. Some need low ESR, some hate it. It all depends.
Some links:

https://www.eevblog.com/forum/beginners/linear-regulator-output-capacitors-ceramic-electrolytic/
https://training.ti.com/ldo-loop-stability-and-transient-response-analysis

Just stick to the datasheet recommendations for your LDO board, and add any additional caps as needed on the breadboard. There are so many potential causes for disturbances coming from the circuit on the breadboard, no need to overthink your LDO board.

But don't over-trust your USB input power quality. There are some shoddy ones out there. You may not want to go all in with something like a STBP112, but I'd really suggest at least a TVS (like a SMBJ5.0A) plus a PPTC fuse.

[ilium007]

Thanks! If I use the TVS is it placed on the VBUS input line between VBUS and GND?

[mariush]

I don't recommend 1117 regulators ... some require a minimum ESR on the output, like 0.1 ...1 ohm ESR , so the datasheets recommend tantalum or electrolytic capacitors instead of ceramic capacitors.
The dropout voltage doesn't matter, your input is 4.5v..5.5v so you have at least 1v between input voltage and output voltage ... lots of LDOs out there that need less than that to work right.

I would recommend using other packages like SOT-223 or DPAK / TO-252 which have a larger surface to dissipate heat into the pcb, and basically use a copper area around the chip as a radiator. Besides a decoupling capacitor (0.01 / 0.1 uF) close to the input voltage pins, linear regulators aren't that sensitive about how close the capacitors (or diode or inductors in case of switching regulators) so you can have a small area of just copper around the tab of a regulator. 

For example, in the AP2112K datasheet, the thermal resistance for the SOT25 version which seems to be the one you use, is 184 C/W

You'll have 5v input, and you have 3.3v output, so at 0.5A of current output, chip's gonna dissipate (5v-3.3v) x 0.5 = 0.85 watts. So if the chip were to be floating in air, with just wires soldered to it, it would get very hot. Soldered to pcb, it would dissipate some heat through traces but not that much ... so at 0.5A it would be quite hot.

Even UFDN package is a tiny bit better at around 173C/w - for example Microchips MIC5528 (MIC because it was made by Micrel which was bought by Microchip) 3.3v 500mA regulator is better: https://ww1.microchip.com/downloads/en/DeviceDoc/MIC5528-High-Performance-500mA-LDO-in-Thin-and-Extra-Thin-DFN-Packages-DS20005982B.pdf

But here's some other suggestions

Microchip TC1262 : fixed 3.3v at 500mA max, dropout voltage 650mV at 500mA, 59 C / w on SOT-223  :  https://www.digikey.com/en/products/detail/microchip-technology/TC1262-3-3VDBTR/443194
See page 4 of datasheet for thermals discussions : https://ww1.microchip.com/downloads/en/DeviceDoc/21373C.pdf

Microchip MCP1825T-3302 : fixed 3.3v at 500mA , dropout voltage, dropout voltage around 210mV at 500mA, around 32C/w on  DPAK : https://www.digikey.com/en/products/detail/microchip-technology/MCP1825T-3302E-ET/1635463

And there's lots of other chips, and you could also go for adjustable versions, and simply add footprints for two extra resistors to set the output voltage. Surface mount resistors are cheap.

As for the layout, you have lots of space on that board, take advantage of that... use thicker traces, use larger copper areas...
The two resistors by the usb connector can be rotated 90 degrees and shifted down a bit out of the way, so you can have the 5v line directly out of the connector to the right 
The linear regulator can then be oriented so that the output goes towards the top of the board and you can get the ceramic output capacitor between the 6pin header and the regulator.
Thicker trace can go along the bottom side of the board to the other regulator.
You can totally do this without jumping to the bottom layer.  Worst case scenario, add a 0 ohm jumper link / resistor to your schematic. so you can jump over a trace and not use vias to break the bottom which can be whole ground fill.

Oh I'd also align the 3 pin header with the 6 pin header on the right, and put the text to the left of the header, just to have all pins align.

You could also move the power on led between the two headers on the right, if you think it would be a better place (if it won't be obstructed by wires)


I made a mockup of the left side, but again, ideally you'd use a larger footprint regulator on the board for better thermals.





 

[ilium007]

Thanks - I'll go through all of the points in your response when I have time to digest them properly. I need more than 500mA for the ESP32 which is what I am putting together a power supply for (after I build this breadboard supply) so I will need to find something in a DPAK / D2PAK case with high output current.

[bateau020]

Thanks! If I use the TVS is it placed on the VBUS input line between VBUS and GND?

You typically do something like this (the fuse will protect the circuit and will trip when the TVS kicks in):

[ilium007]

hehehe I was on the right track, I need to change mine diagram to use the uni-directional TVS! From what I am reading the selection of PTC / TVS is another minefield.

Now I need to find a better voltage regulator.

[bateau020]

About the 6 pin headers that you use to plug in the breadboard: The pins are too close together to avoid the board from being tilted and get loose when you touch it, and it will be relatively hard to plug it into a fresh board. You could try 2 times 2 pins, spaced out a bit:

[ilium007]

Will do.

[mariush]

You can find ADJUSTABLE linear regulators that can do more current .. 0.8A .. 1A is typical for SOT-223  and 2-3A is possible on DPAK  (see for example *1084  and *1085 linear regulators)

For fixed linear regulators, the selection is smaller.

USB on computers gives you 5v at 0.5A for USB 2.0 ports,  5v at 0.9A for USB 3.0 ports, but most computers don't limit the current on individual ports.  At best, computers will have a reset-able fuse set somewhere above 2A of current for each pair of usb ports on the back of your computer.  So, you could probably get nearly 2A of current from the usb port.

Linear regulators take the input power and output a lower voltage, but they dissipate (throw away) the difference as heat.  So if your usb input can do maximum 5v at 1A for example, you have 5W in, but your linear regulator won't output more than 1A of current, minus what it consumes internally to work (around 1-5mA for cheap linear regulators) ... so you have 5W in , 3.3W out.

If you want to power things like ESP32, according to this page - https://lastminuteengineers.com/esp32-sleep-modes-power-consumption/ -  it peaks at around 260mA when it transmits and everything is turned on,  so a 500mA LDO should still be fine.
But, if you want higher efficiency and not waste 1 watt of power, you'd want to use a switching regulator instead, these can be up to 95% efficient and generate very little power.

There are modern designs which are very easy to use and only require an additional inductor, but they require very careful layout

Have a look for example at MIC23150 that can do up to 2A of current, here's the fixed 3.3v out version : https://www.digikey.com/en/products/detail/microchip-technology/MIC23150-SYMT-TR/1974106

Or have a look at MIC2230 ,  DUAL  adjustable  2 x 800mA : https://www.digikey.com/en/products/detail/microchip-technology/MIC2230-AAYML-TR/1834671
See page 17 of datasheet for example circuit where both outputs are set to 1.8v (but you can change the resistor values to get 3.3v)

Or something in a more basic footprint, easier to solder by hand, AP6502 : https://www.digikey.com/en/products/detail/diodes-incorporated/AP6502SP-13/2767804
Or AP3401 : https://www.digikey.com/en/products/detail/diodes-incorporated/AP3401KTTR-G1/6186982

[ilium007]

I will be powering projects from a Raspberry Pi USB-C power supply capable of 5.1V 15.3W.

https://core-electronics.com.au/raspberry-pi-4-official-power-supply-usb-c-5v-15w-white.html

So 3A output is available. My experience with brownouts on the ESP32 tells me I need an LDO with more than 500mA output.

The regulators suggested above are buck devices which I don't want to try and understand at this point, I was hoping to just use an LDO regulator.

[tooki]

My suggestions:
* thermal relief is not really needed if you hand solder, not on this type of circuit.

Huh? Hand soldering when surrounded by a big ground plane is precisely when you need thermal reliefs the most! Without them, the ground plane sucks away the heat, which you’re introducing from exactly one point, the soldering iron tip. It can make hand-soldering them extremely difficult, especially if there’s also via stitching nearby. And the added time this difficult soldering can take is added time the component is under direct, uneven thermal stress.

Given that thermal reliefs make hand soldering easier, and prevent tombstoning when reflowing, there’s no reason not to use them most of the time.

[bateau020]

My suggestions:
* thermal relief is not really needed if you hand solder, not on this type of circuit.

Huh? Hand soldering when surrounded by a big ground plane is precisely when you need thermal reliefs the most!

Let's say it depends on the skill, the size of the components, the sensitivity of the components to thermal stress, and the power and type of the soldering iron. For this circuit it can very well be done without. Just pre-"wet" one pad, and off you go. There are indeed cases where thermal relief would be needed.

[Ian.M]

I'd want two 3.2mm mounting holes in the corners furthest from the breadboard, with clearance for a M3 nut either side so you can use two longish M3 machine screws as legs to support it at the correct height for your breadboard, without wasting breadboard area.

A polyfuse inline with the 5V rail is essential.

I'd want separate voltage selection jumpers for each side of the breadboard, and also a female header to pick up 5V, 3.3V and Gnd, for occasions where you have both sides set to the same voltage, but need the other voltage for just one part of your circuit.

A power switch would be nice.

Also why not break out the USB 2.0 data lines D+ and D- to a female header (+Gnd) for occasions when you have a USB capable MCU on your breadboard?  While signal integrity is unlikely to be good enough for Full Speed (480Mbps), High Speed (12Mbps) and Low Speed (1.5Mbps) typically work OK, especially if you twist D+, D- and Gnd together between the USB connector and the MCU.  A specialized USB protection TVS diode array would be a worthwhile addition to give the data lines some protection against ESD and breadboarding mishaps.

[bobbydazzler]

I've found what looks like a better LDO regulator....

LDL1117  https://octopart.com/ldl1117s33r-stmicroelectronics-81876163?r=sp

Much lower dropout voltage of 350mV at 1.2A. I am still confused by these input and output capacitors. The datasheet shows 'typical' input / output capacitor values and it says that I can use ceramic capacitors. Do I just go with the 1uF / 4.7uF values? Surely I have to consider the transient loads involved? This breadboard is just a test circuit for a 3.3v supply I will use for an ESP32 based project.

(Attachment Link)

The stability graphs seem to indicate that for very low ESR (assume thats what my MLCC will be given there are no ESR specs documented in their datasheets) a 22uF is best.

(Attachment Link)

Looks like as long as esr is <6ohms you should be fine.  I would use mlcc anyway for this(at least on the input) and if the ESP32 load needs more capacitance add it to the input of the ESP32 not the output capacitors for your LDO.

[tooki]

My suggestions:
* thermal relief is not really needed if you hand solder, not on this type of circuit.

Huh? Hand soldering when surrounded by a big ground plane is precisely when you need thermal reliefs the most!

Let's say it depends on the skill, the size of the components, the sensitivity of the components to thermal stress, and the power and type of the soldering iron. For this circuit it can very well be done without. Just pre-"wet" one pad, and off you go. There are indeed cases where thermal relief would be needed.

That’s a whole lot of “ifs” for when you can get away with not having reliefs. The OP is a beginner, so probably not super high skill. They’re unlikely to have a high-performance iron. Most of the components in question are capacitors, which are sensitive to thermal stress (to the point that manufacturers recommend not hand soldering them at all!), especially one-sided stress.

I work at a training center, and have beginning electronics apprentices all the time. Components on ground planes without thermal reliefs are a constant source of difficulty for them. (And that’s with good JBC irons.)

As for “pre-wetting” one pad: uh, that’s the standard way to hand-solder chip components regardless of thermal reliefs.

[bateau020]

I work at a training center, and have beginning electronics apprentices all the time. Components on ground planes without thermal reliefs are a constant source of difficulty for them. (And that’s with good JBC irons.)

Understood. Fair point. Thermal reliefs are safer.

[ilium007]

There are modern designs which are very easy to use and only require an additional inductor

I have spent hours today going through datasheets, I think I need to start looking at the switching buck converters. There is just nothing in stock anywhere, let alone the supporting passives (1 x 10uF 3A inductor in stock at lcsc.com). I didn't know that this component shortage is as dire as it is.

I did however find the the Torex XC6220 that look quite good for a linear regulator. Available in 3.3 and 5.0 fixed outputs and works with ceramic caps - https://www.torexsemi.com/file/xc6220/XC6220.pdf

[ilium007]

These Diodes Inc switchers look good - https://www.diodes.com/assets/Datasheets/AP63200-AP63201-AP63203-AP63205.pdf

AP63203 / AP63205 are the fixed 2A 3.3V / 5.0V output versions.