I am currently working on a project and I have designed a schematic and the corresponding PCB. I would greatly appreciate it if you could take a look at my design files and provide any feedback or suggestions for improvement.
Thank you in advance for your time and help.
āLittle boxes, little boxes, and theyāre all made out of ticky-tacky, and they all look just the same.ā
I hate that kind of schematic design. But I know itās fashionable now.
Typically you can click at picture and see it bigger. I donāt know why I canāt see your pictures enlarged.
These are .SVG files and unfortunately web browsers have been extremely slow in implementing that standard, and apparently also not much effort is put into web browsers (frameworks) to show them at different sizes etc. Quite a shame because I quite like the .SVG vector format. The schematic has āBoard1.svgā as filename. This is not a very meaningful filename.
For the schematic. I donāt like the blue boxes around all schematic sections. It does nothing what a bit of whitespace does not do and itās an extra bore to maintain them. Sometimes these can be useful to put a bit of emphasis onto something special, but not for all sections. I do like the use of titles above schematic sections, but normally draw them in a lot bigger font. Both to put more emphasis on the titles, and to make them readable when zoomed out.
The schematic symbols are also āweirdā at best. For most, they do follow common conventions (voltages top - down, and signals from left to right), but the wide bodies take up a lot of space. U16 also does not follow this convention. Putting pins in pin number order on the schematic is a bad practice. Schematic symbols should be designed to display itās function.
What does the ā/NOPBā mean in the schematic symbols? They appear to be part of the reason the schematic symbols are so big. Usually texts are placed just outside of the symbols, so the boxes can be made much smaller.
Why didnāt you just use KiCadās native symbols for the LM1117?
(Also see PCB remarks below).
700 Ohm (R21, R22, R23) in series with a power supply output?
There are also two sections that are implemented twice. KiCad has āhierarchical sheetsā for this. Basically you just draw such a circuit once in KiCad, and then include two copies of the sheet it is on. This makes maintenance easier, because with hierarchical sheets, the copies will always be the same. Even if you for example change a 5uF capacitor for a 4.7uF capacitor.
For the PCB. It only shows a single layer. I do see some test points, but no viaās.
Pin mapping to the SOT223 devices (LM1117) looks wrong. Pins 1 and 2 should not be shorted. You also used thermal reliefs for the big ātabā pins, while these are supposed to be soldered to some copper to act as a heatsink.
It looks like you put some effort in the PCB layout itself, but itās hard to see whether the decoupling capacitors are placed properly. Yellow text on red and white background is also hard to read, especially with the very thin and small texts. These texts also look too small to be readable as silk screen text.
How do you want to connect the outputs? Soldering wires to those small SMT pads is a nuisance.
Iām not a fan of the blue boxes eitherā¦ I like schematics to have actual wires connecting actual signals, except for power/ground.
The ānormalā schematic way is to use āspecialā symbols for power and ground. Youāve used an appropriate ground symbol, why not use the power symbols for each power rail instead of global labels?
also, itās common practice/old school to avoid 4-way junctions on wires. I would change this spot on your schematic.
The layout image is a bit small but two other āstyleā/common things to avoid are Y junctions and 90 corners on signals.
Try to go from one pad to the next, instead of going at right angles.
also, since this is a power board I would think that on your power outputs you might want thicker traces to supply more power with less loss/resistance in each output.
Agree.
I believe the purpose of wires is to join components. It is oh so much trouble to hunt around a small schematic such as this to find what little box is supposed to connect to what other little box. 
I cannot seem to get a big enough view of the schematic to read easily.
But maybe 2-3 years ago on this forum there was an excellent comment about a āschematic diagramā which used an excess of netlist connectors instead of wires. The comment called it a āgraphical netlist.ā I thought that was highly appropriate.
Around 3 a.m I was not clever enough to find it 
After downloading these files at my HDD I can open and see them enlarged.
I have never used and will never use such way of schematic drawing, but let anyone do as he likes to.
U16 function is hard to understand. Pins 4,5 should be on the left, 3 on the right, 1,2 at bottom.
I think āNoPbā = āPbFreeā. When RoHS directive came it did not apply to all products. If company manufactured devices falling under RoHS and not they have to distinguish the same elements being RoHS and not so they need separate symbols for them. This may be a remnant from those times.
I donāt think it is a power supply. It is rather high voltage source. May be for varicap diodes polarization.
Extreme filtering suggest it.
For LMP2021 I would rather use standard OpAmp symbols - it would be clear what it is when reading schematic.
Very surprising are 10nF, 1nF, 50pF electrolytic capacitors !
It looks that there is intention to well filter U16 output. I would think about adding ceramic capacitor in paralel to each electrolytic capacitor as ceramic capacitors have much, much lower ESR and ESL.
This filter is a kind of circuit I would simulate with Spice using the as good as possible capacitor models (including ESR and ESL) to find what is really needed and what not.
Simulate parallel connection of ceramic capacitors with different capacity (as they are at the filter end) using their models including ESR and ESR. You will see resonances between them. For ceramics having very low ESR (around 0.01Ī©) this are high resonances. If disturbance will hit this frequency it will be strengthened, not suppressed (not a big problem here thanks to R21ā¦R23 being used).
Connecting ceramic in paralel with electrolytic is not a problem because high electrolytic ESR dampens resonance.
In filters before and after DCDC converters I use 0603 ferrite beads having 0.3Ī© DC resistance and 1kĪ© impedance at 100MHz. You can get Spice models from Wurth. Unfortunately simulation of them is not close to reality. In real they resonate less than you get from simulation. It is because models use elements with their values independent from frequency while really losses in such ferrites increase with frequency.
And about PCBā¦
If Capacitors are supposed to filter switching regulator noise it is better to go with tracks through their pads (like C20) but not have them connected with separate track (like C17, C19, C22, C23, C24).
I hope your output pads are THT (have plated hole in them).
My PCBs are for analogue circuits, no more than 100mm x 100mm and are all hand-soldered. So my component pads will tend to be larger rather than smaller, and so will the tracks. Whilst I ground-fill both sides of the board, I will make sure my power distribution tracks are nice and wide, with 100n caps next to every component!
I studied electronic engineering at university far too many years ago, and the emphasis was simply on ājoining the dots correctlyā, with little or no information given about PCB design, and power distributionā¦ which is a shame, because without both of those, your fancy circuit, whilst correctly connected, simply might not work. I guess back then, with CPU speeds being only 1 or 2 MHz then the strange effects of noise on signals was less important.
May be the widespread availability of mobile phones have even bigger influence. If remember well cell phone can generate 1V/m field at 1m distance from it (have to be strong as its signal should be receivable by a base station at even 5km distance).
I saw that as well. However I always added additional information to communicate the subtleties of some of the circuits. For some reason folks fought me (to no avail).
Another interesting thought (not too much on schematics but more mechanical). What if you are forced to design in an non optimum way due to patents that donāt allow you to do the same in a better way?
Regarding the MAX5025 chip you have followed the application note for the 30v variable output almost to the letter, may I ask why the extra filtering has been added and has this filter been tested please, if so what are the results or expected results ? 
just curious 
