As the sibling comment mentions there are several aspects.
You'll need proper input filtering which may require a non-trivial filter network. You'll also need proper output filtering, which does include slapping a lot of capacitors on there, but also careful selection of those capacitors both type and size. Parasitic inductance of larger packages can mean they can't filter high frequencies, and MLCC capacitors have a DC bias which means the effective capacitance is significantly reduced when they have a DC bias on them which they will have in a DC-DC converter.
Then you need to take great care about component placement and board layout, to minimize the return path of the currents and such.
You can skip all of that and get a board that functions as a DC-DC converter if you measure it with a multimeter, but actually be horrible. And you just can't fix bad layout by slapping more capacitors on there. And even with a not terrible layout, you can't fix it by using the wrong kind of capacitors. Like anything through-hole is just not gonna pass.
I think a lot of people are overly cautious of DC-DC conversion in this topic, but you've gone full-tilt in the opposite direction and are severely underestimating the problems that occur.
1. Its not "power-conversion" that's hard per se, its EMC that's very hard and not taught very well at a bachelor's level.
2. DC-DC Voltage Converters usually handle the entirety of your board's power, meaning they are the highest power component.
3. High power and high-frequency is a difficult EMC problem. This means that a bad design will absolutely send your electrons / energy out and radiate out like an antenna. And if things on the same board pick it up, it will be called crosstalk. And if things off-board pick it up, its called electromagnetic interference which almost certainly leads to a compliance problem.
---------------
1. Hobbyists don't care about compliance. So bam. We are already dealing with the biggest problem by simply not caring about it. (Maybe you can care and go into deeper studies, but... if you're a beginner just don't care. Learn this very difficult stuff later).
2. Prevent crosstalk by following good board design rules: have a 4-layer board. Use Power+Signal / GND / GND / Power+Signal stackup. Use two vias (one for signal-1 to signal-4 traversals), and a 2nd via for GND2 to GND3 traversal of the return current). Thinking of both the forward current and a tightly bound reverse current is basically all you need to do to avoid difficult crosstalk problems on board.
Done.
Point#2 requires deeper studies than is typical in bachelor's level electrical engineering. But it truly isn't very difficult once you learn the theory. Tight ground-planes reduce crosstalk (and EMI problems), and furthermore thinking of the return-current explicitly prevents problems.
Now you could have some truly difficult "ringing" from trace inductance and other such nasty problems... but that tends to occur beyond 100MHz. I'm thinking most beginners are going to be under 20MHz for most of their designs and thus never deal with those advanced "PDN" / Power Delivery Network problems.
Though if you do go into PDNs, its obviously a tough subject with huge amounts of study and reading involved. But most of the problems truly are at very high frequencies and/or at EMI compliance. Beginner Hobbyists avoid the most difficult issues entirely by nature of beginner (aka: low-speed) and hobbyist (and therefore don't have to follow regulators).
----------
I'm not a professional. But my understanding is that top-level EEs who work on PDNs will simulate the circuit-board itself to figure out trace inductances / capacitances in the board itself. (Closer planes of ground/power will create more capacitance. Long traces tend to increase trace inductance, etc. etc.). And tight simulations are the only way to truly understand the PCB and how it interacts at high frequencies with high-power.
But such methodologies are gross overkill for a 1MHz boost converter with a pre-made PCB Layout, and a list of capacitors + inductors already picked out for you. (ex: https://www.microchip.com/en-us/product/mcp1640)
We have a couple of challenges today. Hobbyists often go over 20MHz, because they put WiFi, BT or USB on their boards, giving EMC issues. Also, the speed of the modern ICs tend to be very high. If you have a 9600 Hz UART signal, that is not a 9600 Hz signal if it's a square wave with a modern IC with very short rise time on the pins. So a good old, slow serial line can with modern MCU emit noise up in the hundreds of MHz range.
So your PCB layout tips are important, even on slow circuits these days.
Depends on your definition of beginner. It's trivial to put a nrf52 module (like [1]) in a PCB design and wire a USB socket to it; just make sure to route the data lines as a differential pair in kicad (add protection diodes if feeling fancy). And speak a little prayer that it actually works as intended. No need to understand what any of that means.
Of course the notion of using such a module might be a step up from beginner for you, but IMHO it's more about the understanding. But I agree that there is no definite definition.
> Use Power+Signal / GND / GND / Power+Signal stackup.
I'm just a novice (maybe intermediate) so I'm wondering: the common 4-layer stackups available to hobbyists seem to be 1oz/0.5oz/0.5oz/1oz and I assume the outer layers have better thermal dissipation since they're only kept from the air by solder mask; so wouldn't it be better to put power/ground on the outer layers and keep signals in the middle?
Also maybe I'm weird and this is pointless but I typically put a filled copper zone tied to ground on every single layer, unless I have a reason to put some other kind of zone in a particular area. Is it necessary to have a full, dedicated ground plane, rather than ground + signal or ground + power?
> so wouldn't it be better to put power/ground on the outer layers and keep signals in the middle?
Signals must never cross a break or split in the plane they're referencing (usually 0V or ""ground""). This creates huge EMI problems. Your proposal would have signals on layer 2 crossing a split in the ground plane on layer 1 (that split caused by power traces).
Ground fill is counterproductive on the signal layer.
If you accidentally get the return path on layer1 or layer4 instead of the designated layer2 or layer3, you've created noise.
Power+Signal / GND / GND / Power+Signal is about consistency and braindead-easy tracking of return paths. The return path for layer1 is always layer2. The return path of layer4 is always layer3.
Keeping track of both the forward signal (or power line) and the reversed return current (which was electrically induced onto the nearest reference plane) stops working if suddenly you have random reference ground-fill planes on the layer1 or layer4.
DO NOT put GND on layer1 or layer4 if you're doing this methodology.
---------------
Beginners likely aren't working with a hot enough circuit where thermal dissipation is an issue. If you do have thermal dissipation then I guess thermal ground on layer1 and layer4 ties with thermal vias will be needed.
In practice, the thermal resistance across the PCB cross section is better than beginners expect anyway. Thermal conductivity is just one attribute, the other attributes of heat movement are distance and cross sectional area.
So the shape favors you up and down the PCB. Yes the fiberglass has worse thermal conductivity but you win on shape.
