V=<skill dir>/view.py
python3 $V sch board.kicad_sch -o <scratch>/sheet.png                    # whole sheet
python3 $V sch board.kicad_sch -o <scratch>/u2.png --around U2,C3       # zoomed to these symbols
python3 $V sch board.kicad_sch -o <scratch>/a.png --zoom 120,30,80,60   # window x,y,w,h (sheet mm); --page N
python3 $V pcb board.kicad_pcb -o <scratch>/top.png                     # whole board, F.Cu + silk + outline
python3 $V pcb board.kicad_pcb -o <scratch>/u2.png --around U2 --layers F.Cu,F.SilkS,F.CrtYd,Edge.Cuts
python3 $V pcb board.kicad_pcb -o <scratch>/bot.png --back              # bottom, seen from below (mirrored)
python3 $V pins board.kicad_sch U2 R3                                    # each pin's net (no refs: every part)
python3 $V net board.kicad_sch /I2C_SDA                                  # every pin on a net
python3 $V ohms board.kicad_sch +3V3 [GND]                               # resistance between nets, resistors only
python3 $V expect board.kicad_sch DESIGN.md                              # check stated connections
python3 $V decoupling board.kicad_sch                                    # each IC supply pin and the caps on its rail

--dpi and --margin adjust the crops. kicad-cli is found at its usual place on macOS and Windows, or on PATH, or from $KICAD_CLI.

Connections come from the netlist, not the picture. A wire that looks connected but isn't shows up as its own net: a missing junction, a label one character off, or an end one grid step away. Unnamed nets read Net-(C2-Pad2); unconnected pins read unconnected-(U1-NC-Pad5). Names escape / as {slash}.
ohms solves the resistor network between two nets (capacitors open, ICs and diodes ignored), lists the other parts across both nets, whose leakage or clamps can change a meter reading, and lists series chains of two-pin parts that aren't all resistors (an LED and its resistor): give those both meter polarities. Values read like KiCad's (4k7, 10k, 1M, 100R; m is milli).
expect reads every line shaped like `U2.4 = +3V3` (pin on a net) or `U2.4 == C3.1` (two pins on one net) from any file, such as a list in DESIGN.md, and reports each mismatch. Exit code 1 on a mismatch or when no line matched.
decoupling lists each IC's power_in pins by rail with the capacitors from that rail to ground, and flags a rail with none. Exit code 1 if any.
Pictures are for spotting problems. Take numbers from the files or from board.py pads.
Overlap: judge text overlap only from a zoomed crop. A whole sheet is too small.
Layers: use canonical names (F.SilkS, F.CrtYd, In1.Cu). One copper layer per picture, since a bottom pour hides top tracks.

3D render

K is kicad-cli: /Applications/KiCad/KiCad.app/Contents/MacOS/kicad-cli on macOS, C:/Program Files/KiCad/10.0/bin/kicad-cli.exe on Windows, kicad-cli on Linux.

"$K" pcb render -o <scratch>/3d.png --side top --quality basic --width 1600 --height 1000 board.kicad_pcb

Add --zoom 4 --pan "X,Y,0" for a close-up (aim by trial), and --side bottom, --perspective or --rotate for other views. Parts without a 3D model (some sensors) show only their pads.

Compare two revisions

mkdir -p <scratch>/old <scratch>/new
git archive <old-rev> | tar -x -C <scratch>/old       # or use the working tree as "new"
git archive <new-rev> | tar -x -C <scratch>/new
for t in old new; do python3 $V pins <scratch>/$t/board.kicad_sch > <scratch>/$t.tsv; done
diff <scratch>/old.tsv <scratch>/new.tsv

Changed lines are pins whose net changed.
Auto-named nets (Net-(...)) rename when their namesake part changes. Check them, but they aren't necessarily changes.
Values and fields: run "$K" sch export bom --fields 'Reference,Value,Footprint,${DNP}' -o <scratch>/$t.csv <scratch>/$t/board.kicad_sch for both trees and diff the two files.
Pictures: plot the same area from both trees and compare them side by side.

kicad-view

Look at a KiCad design