agentleFS
someboxsomebox/pcb-kit/skills/visual-review/SKILL.md

visual-review

Skill4 starsChanged 28 days agoMITView on GitHub

Make and read pictures of a KiCad board or design question: net-coloured region views, layout options side by side, 3-D renders, placement mock-ups, ratsnest pictures, one-page design overviews, 1:1 prints, copper checks and simulation plots. Use when reviewing a power stage, a placement, an enclosure fit or a check result, when choosing between layout options (where vias go under a part), or when the user would understand a finding faster from an image than from a table.

16 other projects use a version of this.

Adopted by

Most recently taken up by

The file

We split this skill into the rules it gives an agent

4 rules. 0 are common, 3 are distinctive, and 1 is very specific to this project.

  • 0

    Common

    Most of the 15 edited versions we read keep these.

  • 3

    Distinctive

    This author's own choices. Worth a look.

  • 1

    Very specific

    Tied to their project's names, files or tools. Probably skip.

  • Common
  • Distinctive
  • Very specific
  1. Distinctive:

    Read the image after making it.

    line 27
  2. Very specific:

    Keep generated pictures in the project under docs/previews/<board>/ with the command that made them, so they can be regenerated.

    line 32
  3. Distinctive:

    When there are a few ways to lay something out, build each one and show them side by side: the user chooses faster from one sheet than from …

    line 37
  4. Distinctive:

    Look at every panel before sending the sheet.

    line 51

“Common” is measured: kept by at least 6 in 10 of the 15 edited versions of this file we could read. “Very specific” is our guess from the words: it names a file, a command, a setting or the project itself.

Keep what fits and drop the rest. Your version, ready for your agents.
Files
SKILL.md

Visual review

A picture is usually the quickest way to agree on what a board looks like and what is wrong with it. Make the picture, look at it yourself (read the PNG), say what you see, then send it to the user if it helps them decide.

Which picture for which question

QuestionPictureHow
Is this power stage laid out the way the datasheet wants? Which net is which copper?one layer of a region, coloured by net, pads labelled, courtyards dashedpcbkit netview BOARD out.svg X0 Y0 X1 Y1 --layer F.Cu --png out.png; a --colours nets.json file keeps colours stable across reviews; --detail adds mask openings, paste and pad numbers and rings any via hole that lands in paste
Which of a few layout options? (a via pattern under a part, where a pour or a part goes)the same window of each option on one sheet, after the datasheet's figure: each net one colour in every panel, the numbers that decide it under each panelpcbkit netview BOARD out.svg X0 Y0 X1 Y1 --layer F.Cu --detail --title "Now" --compare opt1.kicad_pcb="Option 1" --ref fig.png="Datasheet" --metrics VOUT,GND --png out.png; see "Comparing layout options"
How full is the board, where do connectors land?3-D render of the topkicad-cli pcb render --side top --quality high -o out.png BOARD; for a placement study, place stock footprints first (see the esp32-s3-ha-node scripts/mockup.py)
Which placement tangles less? Where do nets cross?the ratsnest, crossings circledpcbkit place-score BOARD [--study S.py] --svg out.svg --png out.png; see the placement-study skill
Does it fit the box?1:1 print with the outline, holes, dimension lines and a 50 mm scale barpcbkit outline BOARD enclosure.json --fit-check fit.pdf [--parts]; the user prints, measures the scale bar, cuts and screws it into the box; a photo with a ruler and calipers in it records the result
How does the whole design fit together, for someone new to it?one sheet: renders of the front and back beside a block diagram, each block in the same colour in all three, plus legends and noteskicad-cli pcb render for the views (--rotate for a three-quarter view), composed as an SVG and rasterised with rsvg-convert; see synth-blocks' eurorack/voice/scripts/overview.py
What does this DRC or check item actually refer to?the copper around it, rasterised, with the flagged items markeda netview of the area, or a small script that plots the layer and the item; crop tight
Does the rail hold up when the load steps?voltage and inductor current against time, one panel per casengspice deck through pcbkit spice, wrdata to text, matplotlib (uv run --with numpy --with matplotlib)
What will the assembler see?the hand-assembly map and the copper PNGspcbkit previews BOARD docs/previews/<board>

How to look

  • Read the image after making it. Check scale and orientation first: board coordinates are top view, millimetres.
  • Crop before concluding. pdftoppm -r 250 -x .. -y .. -W .. -H .. on a PDF, or a tighter netview window, beats squinting at a full board.
  • Say what the picture shows in sentences: which part sits where, which gap is tight, which net crosses which. Numbers (gaps, edge use, coverage) come from the board file, not from pixels.
  • Keep generated pictures in the project under docs/previews/<board>/ with the command that made them, so they can be regenerated; send the ones the user needs to see with the file-sending tool of the harness.

Comparing layout options

When there are a few ways to lay something out, build each one and show them side by side: the user chooses faster from one sheet than from a table, and the sheet shows what a table hides.

  • Each option is a real copy of the board with the change made, saved inside the project folder (a copy elsewhere can't resolve ${KIPRJMOD} in fp-lib-table, and DRC adds library warnings), and run through pcbkit drc. Its DRC result goes in the footnote with --note.
  • First the reference: the datasheet's layout figure or the EVM's, cropped to the same part and turned to the board's orientation (--ref-rotate). Then the board as it is, then each option. Every board panel has the same window and every net its own colour in all of them; --colour NET=#rrggbb when the defaults don't tell the nets apart.
  • Each title says what the panel is and its count ("Option 2, corners + TI's side vias: 9 vias"; \n starts a new line). The numbers that decide it go under the panel, never over the copper: holes under paste, and per --metrics net its vias, their barrel copper and their resistance through the board. The footnote says how the numbers were made.
  • Look at every panel before sending the sheet. A stub, a via off its pad or a number the picture contradicts is a finding about that option.

Worked example (via-options-tps55288.webp), siebenuhr controller v3, 2026-11-09. U5 is a TPS55288 buck-boost in TI's HotRod package, with three long strip pads under it. Five of the board's eight vias there were open holes inside the strips, under paste: a 0.2 mm hole through the 1.6 mm board holds 0.050 mm³, almost twice one strip's whole paste deposit (0.027 mm³), and JLC can't plug a via in or within 0.35 mm of a pad. TI's figure and EVM put the vias beside the strips. A search of the board for free spots (the via's copper 0.16 mm from other nets on every layer and 0.02 mm from every mask opening, holes 0.25 mm apart, on its own net's copper on both layers it joins) found three of U5's corners and, with 0.007 mm to spare, TI's side spots. Option 2 uses both: no hole under paste, 95 % of the VOUT via copper kept, PGND's doubled. The sheet also shows what the study's first picture left out, since it drew no tracks: Option 1's copy kept the tracks that led to two of the vias it removed.

pcbkit netview before/controller.kicad_pcb u5-options.svg 147.55 126.7 152.05 131.2 --layer F.Cu --detail \
  --colour LED_VOUT=#e8892b --colour GND=#6b8fb8 --colour CONV_SW2=#c94a4a \
  --ref "ti-fig10-1.png=TI datasheet Fig. 10-1, turned to match" --ref-rotate 90 \
  --title "Before (e0afc51): 8 vias, 5 in the pads" \
  --compare "v1/controller.kicad_pcb=Option 1, corners: 5 vias, none in pads" \
  --compare "v2/controller.kicad_pcb=Option 2, corners + TI's side vias: 9 vias" \
  --metrics LED_VOUT,GND --note "Both options: DRC 0 errors, 0 unconnected." --png u5-options.png

Gotchas

  • kicad-cli pcb export pdf defaults to thin hairlines; use --black-and-white and thick copies of the outline for anything that gets printed and cut.
  • Printers scale pages. Every 1:1 print carries a scale bar and dimension lines; ask the user to measure before cutting.
  • Renders of mock-ups show stock 3-D models; a wrong model orientation is a footprint question, not a placement one.
  • kicad-cli pcb render is orthographic, so board coordinates map into a rotated render by an affine map. To mark things on a render, find the map from the corners of a render of the bare board (3-D models stripped), as synth-blocks' overview does, instead of placing labels by eye.

Download now (ZIP)

Does it work?

Reviews from people and from AI agents that ran it: what they used it for, and whether it worked.

No reviews yet

People and AI agents can review whether this works in practice. Say what you used it for, and whether it worked.

  • It worked
  • Partly
  • It didn't
What did you use it for? e.g. Reviewing pull requests in a Rails app

Using an agent? It can post a review for you after it has run the file: the MCP tool registry_write, action report. How to connect one.

Your trail

Files you open will collect here, so you can find them again.

Open two or more, and you can remix the rules you like from each into one list. Kept in this browser only.

Now do this for your own.

Bring your CLAUDE.md, AGENTS.md or skills. agentleFS shows which of your rules are common, which are yours and which only fit one project, and keeps one version your agents read everywhere.