boom-vitt/kicad-thai/kicad-pcb

KiCad PCB design (Thai industry)

Reply in Thai when the user writes Thai; keep tool names, layer names and commands in English. Thai engineers mix both ("ลาก trace", "เช็ก DRC"), so references/glossary-th.md maps the Thai terms people actually type to KiCad terms.

0. Look before touching anything

1. Find the project: *.kicad_pro with matching .kicad_sch / .kicad_pcb.
2. Find KiCad: kicad-cli version (macOS: /Applications/KiCad/KiCad.app/Contents/MacOS/kicad-cli,

Windows: C:\Program Files\KiCad\<ver>\bin\kicad-cli.exe, Flatpak: flatpak run --command=kicad-cli org.kicad.KiCad). The bundled scripts find it automatically.

1. Read the file header (version YYYYMMDD) and (generator_version "9.0") to

know which KiCad last saved it. Newer KiCad saves files older KiCad cannot open. Never re-save a project in a newer major version, or tell a team on KiCad 9 to "just open it in 10", without warning them. Details: references/kicad-versions.md.

1. If the project is a git repo, check git status first so every change you make is reviewable.

1. Editing KiCad files safely

KiCad files are S-expressions and the GUI rewrites them on save. Prefer, in order:

1. kicad-cli for anything it can do (checks, exports, upgrades) — read-only on sources.
2. Instructions for the user in the GUI for layout and routing. Routing is

visual work; describe what and where (net, layer, width, which side of a part) rather than generating thousands of coordinates.

1. KiCad's Python/IPC API for bulk, repeatable changes (rename refs, set

fields, place parts on a grid) — see references/kicad-versions.md for which API your version has.

1. Hand-editing the S-expression text only for small, surgical changes

(a field value, a net class, a text string). Before that: make sure the file is not open in KiCad (a ~<name>.kicad_pcb.lck file means it is), keep a copy or commit, change as little as possible, never invent or reuse UUIDs, then prove the file still loads by running kicad-cli pcb drc / sch erc on it.

2. Workflow

Ask only what you cannot infer. These answers change the design, so get them early:

Schematic (วาดวงจร)

• Use KiCad's stock symbol/footprint libraries first; they follow the KiCad

Library Conventions (KLC). Make project-local libraries for custom parts — never edit the global ones.

• Every placed part needs: Reference, Value, Footprint, and for assembly an

MPN and/or LCSC field. Add these fields while drawing, not at order time: kicad-fab-export turns them straight into the fab BOM.

• Power: drive every power net (PWR_FLAG on connectors/regulator outputs), add

no-connect flags on unused pins, one decoupling cap per supply pin close to it in the schematic order so it is close on the board.

• Annotate, then run ERC (kicad-check) and fix errors before layout.

Footprints (ฟุตปริ้น)

• Check every footprint you didn't make yourself against the datasheet's

recommended land pattern: pin 1, pitch, pad size, mechanical drawing view (top vs bottom). This is the most common cause of dead first boards.

• For hand soldering prefer 0805/1206 and SOIC; for JLCPCB/EMS assembly 0402/0603 are fine.
• Thermal pads (QFN, DPAK): add vias, decide on solder-paste windowing.

Board setup (ก่อนลากลาย)

1. Pick the fab first, then load its rules: copy the matching preset from

kicad-check/assets/rules/ as <project>.kicad_dru, and set the same minimums in Board Setup → Constraints.

1. Stackup: 1.6 mm FR-4, 1 oz (35 µm) outer copper is the cheap default

everywhere; 2 layers for simple boards, 4 layers (sig/GND/PWR/sig) as soon as you have fast edges, a radio, USB, or a dense MCU.

1. Net classes: Default at the fab minimum + margin, Power wider. Size

power tracks with KiCad's PCB Calculator → Track Width (IPC-2221 based) from the real current and allowed temperature rise, rather than a rule of thumb.

1. Mains boards: add a Mains net class with large clearance and draw the

isolation slot/keep-out before routing anything else.

Layout (ลากลาย)

Guidelines with reasons: references/layout-guidelines.md. The short version: place connectors and mechanically fixed parts → place by signal flow → decoupling caps at the pins → solid ground plane, don't cut it under fast signals → route critical nets (crystals, USB pairs, switching regulator loops, RF) first → power → the rest → pour zones → silkscreen last.

Thai text on the silkscreen (ตัวหนังสือไทยบนบอร์ด)

Needs a TrueType font and KiCad 9+: KiCad 8 silently drops every Thai vowel and tone mark from the Gerbers (verified). How to do it and what to check: references/thai-silkscreen.md.

Checks and handoff

• Run kicad-check (ERC + DRC with fab preset + DFM review) until zero errors,

and explain every remaining warning you decide to keep.

• Run kicad-fab-export for the Gerber zip, BOM and CPL.
• For anything sold in Thailand, run thai-pcb-compliance before the first

production order, not after — moving a mains trace is cheap now, expensive later.

• For "where do I make/buy this in Thailand" questions use thai-pcb-sourcing.

Reporting back

End each step with: what you checked, what you changed (file + what), what the user must do in the GUI, and what is still unknown. Never say a board is "ready to manufacture" unless DRC with the fab's rules passed and the Gerbers were viewed in a Gerber viewer (KiCad's GerbView or the fab's online viewer).