There are some common myths in PCB designing, and I will list some of them:
a. You must use solder mask expansion -- wrong. Modern high quality factories can address solder mask quite accurately, besides, the extra copper area caused by solder mask expansion may cause tomb stoning. I used to use this feature, but now I do not use it anymore, even with BGA packages.
b. You must use relief connects on polygons -- wrong. If the board is small enough, or you have a well controlled temperature profile, the risk of tomb stoning or cold joints caused uneven heat capacity of ground plane is very low.
c. You must not use acute or right angle -- wrong. Despite I only use 135 deg when changing tracks' directions, I do not feel obliged to do so. If I have to use right angle, then I will use it. The main reason for this myth is because in the old days, acid trap in etching process can ruin your day. Nowadays it is not a problem anymore. It also makes RF performance worse, but until you reached 1GHz+, you will not notice it.
d. All digital signals must be terminated -- wrong. A general rule of thumb for digital signal is 1inch/ns, so if your signal's rise time is 2ns, then you can have up to 2inch distance without terminating it. Apparently for sensitive analog signal, this is not a good idea. For digital signal, this is fine.
e. You should better not use the thinnest track width and spacing provided by the fab's DRC rules -- wrong. Most fabs can easily get you down to 0.1mm, and they specify their process to be 0.15mm. They already left enough margin. I use 0.15mm/0.15mm all the time with 0.3mm/0.5mm vias, and none of them have any manufacturability issues.
f. You must follow IPC rules for high current traces -- wrong. IPC rules are designed for worst case -- heavily crowded tracks, poor ventilation, passive cooling, etc. In real world situations, you can have much higher current compared to what IPC spec says. All, I mean 100%, modern high density power electronics violate IPC rules.
g. Many hobbyists hate small SMD parts, especially down to 0402 sizes. In fact, after getting enough practice, I found small SMD packages, including 0402 passives and 0.5mm pitch QFN/DFN/BGA are very easy to handle, and they saves considerably amount of money spent on PCB area, as well as parts (SMT parts are usually cheaper than their THT conterparts).
I'm going to largely disagree - especially in the context of "this is for a beginner"
a) Soldermask expansion is simply a ratio of soldermask aperture to pad dimensions. Do you mean to tell me you don't have soldermask on your PCBs with BGAs? I don't think so.
b) Relief connects serve a particular purpose, and whilst your statement under standard reflow techniques in commercial CMs may prove true, for hand soldering relief connects are preferred to alleviate micro-cracks, and to simply make hand soldering easier.
c) Again acute and R/A traces have their uses, but best practice is to not use them. If you have to, it should be a conscious decisions with an understanding of the signals involved and the impacts of doing so. Any kinks, cause increased current density in the corners, increasing localised dissipation and radiated fields. Typically this isnt an issue, however it is very application dependent.
I have mixed views on digital terminations and these tend to be fluid and specific with the design in question.
d) Trace thickness depends again on the CM and board fabricator. There is often no need to have ridiculously small traces, and for a beginner, which is whom we are doing this for, the likelyhood of them doing BGA design is very remote. If you go beyond the minimums recommended by the fabricator, you need to appreciate that the reliability and yield may go down and the subsequent cost to cover that yield will go up. "Can they?" is a different question to "Will they?", but the issue here is "Should you?"
e) IPC rules for current traces - again the adoption of IPC-anything is a matter of choice. I know for a fact that not all power electronics designs ignore IPC recommendations. Having designed a fair amount of it previously. But as a guideline for a beginner, they provide an easy first step. Deviation is a design decision balanced against other tradeoffs.
f )Package sizes are contentious. Sure they increase available board real estate, but at the expense of ease of maintenance. Unless I absolutely have to, I will always pick leaded parts (QFP etc) over QFN/BGA. Purely from a re-work point of view. This all depends on the rework tools at your disposal of course. I can rework BGAs with a preheater and a hot air station - do I like doing it? Hell no. Getting 300 odd pins soldered reliably is a PITA! For a hobbyist? Pick whatever packages you are comfortable working with. I used to hate 0402s, now I dont mind them, I'll even tolerate 0201s. Would I expect a beginner to rework these? Absolutely not. 1206/0805s sure, 0603's debatable.