---
name: pcb
description: Create, edit, lay out and review native KiCad circuit boards (.kicad_pcb) and their schematics (.kicad_sch) - parts and nets, ERC, placement and routing, DRC, and a review before ordering (fab limits, decoupling, track width for current, assembly and BOM sourcing for JLCPCB, PCBWay or another fab); exports fabrication files, the netlist and BOM, or STEP for enclosure design. Shows boards and schematics in the CAD Viewer.
license: MIT
metadata:
  repository: earthtojake/text-to-cad
---

# PCB design

## Setup

Run the `cad` command (`~/.local/bin/cad` where it is not on your PATH; `cad.exe` on Windows). If
it is missing, install text-to-cad, outside a sandbox or with its permission:

```bash
curl -fsSL https://texttocad.dev/install.sh | sh
```

On Windows, in PowerShell: `irm https://www.texttocad.dev/install.ps1 | iex`. If the CAD app was
only just added, its server may still be starting: try again for up to a minute first. `cad doctor
--check` explains any other failure, changing nothing; `cad doctor` repairs what it reports.

text-to-cad reads a board or schematic itself, so inspecting either, and viewing a schematic or taking
its snapshot, need no KiCad. DRC (`cad kicad_pcb drc`), ERC (`cad
kicad_sch erc`), every export (`cad kicad_pcb export`, `cad kicad_sch export`) and an edit
(`kicad_pcb.edit`, `kicad_sch.edit`) run KiCad's command line, `kicad-cli`,
and its IPC API from kicode, the `kicad` extra (`cad[kicad]`): the `cad` command installs it the first
time a board command needs it (some 100 MB, once; nothing for you to install), and `cad run` gives a
script that edits a board its environment. Showing a board or taking its snapshot needs it too: KiCad
refills the board's copper pours on a copy before they are drawn, so the first board shown starts that
download. `CAD_KICAD_REFILL=0` in the server's environment turns the refill off (no download; set
it as `CAD_KICAD_3DMODELS` below), and the pours are drawn as the file saved them, as they are when the
download or the refill fails. A KiCad you installed yourself is never run. `CAD_KICAD_CLI` can name
another `kicad-cli` (the command line itself, named `kicad-cli`; KiCad 9 or newer, a nightly's for an
edit). It runs headless, with private settings, and never opens KiCad's app; never open a
board in KiCad's app to check it. Its library variables name KiCad's own libraries, never your
variables or KiCad settings: a project's `sym-lib-table` or `fp-lib-table` row that names a stock
library as KiCad's own tables do (`${KICAD10_SYMBOL_DIR}/Device.kicad_sym`,
`${KICAD10_FOOTPRINT_DIR}/Resistor_SMD.pretty`, any major's spelling) reads it in the libraries of the
KiCad you installed (the newest, if several; or the installation whose `3dmodels` folder
`CAD_KICAD_3DMODELS` names): nothing to set. With no KiCad installed, ERC warns `lib_symbol_issues` that
each such library was not found and DRC `lib_footprint_issues` that it is not enabled; a project that
carries its libraries (`${KIPRJMOD}`) needs no KiCad.

kicode's KiCad is a nightly (10.99), so a board or schematic it saves is in the nightly's format, which a
stable KiCad app refuses; viewing and snapshots still work.

## Native files are the source

Edit the `.kicad_pcb` itself, preserving its companion `.kicad_pro`, `.kicad_dru`, libraries and
schematic when present. Reading or displaying a board never writes it. There is no text-to-cad PCB
model, build step, or generated-board ownership marker. A helper script may make a requested edit,
but reread the current file before editing and preserve unknown records and UUIDs. Do not regenerate
an existing project from an incomplete description.

Change a board through KiCad's IPC API in an edit, a `with` block: `kicad_pcb.edit` hands the block the
open board (KiPy's `Board`, as kicode names it: `kicode.board.Board`) and saves it at the block's end
when the block changed it; a block that changes nothing leaves the file byte for byte, one that raises
saves nothing (its exception goes on), and a save KiCad cannot finish leaves every file as it was,
saying why. A board not there yet is made by KiCad, with its project,
and saved. `kicad_sch.edit` does the same for a schematic ([schematic](references/schematic.md#edit-it));
the two of one project, one inside the other, share one KiCad. Run the script with `cad run board.py`,
which gives it the `kicad` extra (kicode: KiPy and a `kicad-cli` with its headless `api-server`); a
`kicad-cli` that `CAD_KICAD_CLI` names without one is refused up front, before any server starts. Import
KiPy's names from `kicode` (`from kicode.proto.common.types import KIID`, `from kicode.util.units import
from_mm`), never from `kipy`: the two cannot share a process. Saving writes the file in the nightly's
format: one from an older KiCad is upgraded, which the run says, and that older KiCad can no longer open
it. Checks and exports of the saved board are calls after the block (`kicad_pcb.drc`, `kicad_pcb.export`);
a STEP or GLB export holds each part's 3D model where the board's 3D view finds it ([board
views](#board-views)), and leaves out, naming them, the parts whose model is missing (or, in a STEP, only in
VRML); `--to dxf` writes the outline and drilled holes, for an enclosure:

```python
from cad import kicad_pcb
from kicode.util.units import from_mm

BOARD = "board.kicad_pcb"

with kicad_pcb.edit(BOARD) as b:       # the board file is the source; the block edits it in place
    power = [t for t in b.get_tracks() if t.net.name in {"+5V", "+3V3"}]
    for track in power:
        track.width = from_mm(0.8)
    b.update_items(power)
    b.refill_zones()
drc = kicad_pcb.drc(BOARD)
if not drc.ok:
    raise SystemExit("\n".join(drc.human_lines()))  # each finding, then FAILED and the count
for kind in ("gerbers", "drill", "pos", "bom", "step"):
    kicad_pcb.export(BOARD, to=kind, out=f"fab/{kind}")
```

An edit states the result it wants, so running it again is harmless: "U1 is at (10, 20)", "the power
tracks are 0.8 mm", never "move U1 5 mm" or "widen the tracks by 0.2 mm". Set absolute positions,
rotations, widths and nets; create an item only when the board does not hold it yet (find it first by its
reference, net or place). A script stopped halfway and run again then ends where one run would.

A board's design starts at its schematic, which says what connects to what: read it, check it with
ERC and look at each sheet ([schematic](references/schematic.md)) before laying out, and hold the board
to it after. For creation or structured edits read [native files](references/board-api.md). For parts and
footprints read [parts](references/parts.md). To place and route a board, read
[layout](references/layout.md): start from the schematic's netlist, place one part or functional
group at a time ([placement](references/placement.md) says in what order and where), route
octolinear by hand (never an autorouter) with widths for each net's current, and check each step with `cad kicad_pcb drc` and a script of the layout's own properties. KiCad's file coordinates are millimetres, **y down**;
footprint-local positions and rotations must be transformed into the board frame. Use a net's
actual pad positions when routing. Check the datasheet's pin numbers, footprint orientation and
connector mating side; a plausible-looking layout does not establish electrical correctness.

## KiCad's own command line

Use the typed commands first (`cad kicad_pcb drc|export`, `cad kicad_sch erc|export`): their results are
the ones the checks and the viewer read. For anything they do not cover, run KiCad's own command line
with `cad run kicad-cli …`: the pinned kicode `kicad-cli` with its own subcommands and flags (`cad run
kicad-cli pcb --help`), no `--with` needed, headless with private settings, its output and exit code
KiCad's. `CAD_KICAD_CLI` does not change which one runs.

```bash
cad run kicad-cli pcb render --side top --rotate -45,0,45 -o tmp/board.png board.kicad_pcb
cad run kicad-cli project downgrade --dry-run --target 10.0 board.kicad_pro   # then -o DIR without --dry-run
```

Most commands write only their `-o`, though kicad-cli may leave a `.kicad_prl` beside a board it reads.
These rewrite the source: `pcb upgrade` and `sch upgrade`, `fp upgrade` and `sym upgrade` without `-o`,
and `pcb drc --refill-zones --save-board`. `project downgrade` exits 2 without writing when the target
cannot represent the board.

## Edit

1. Inspect the saved board with `from cad import kicad_pcb` in a script run with
   `cad run`; record the parts, nets, outline, relevant dimensions and constraints before
   changing it. [Checks](references/checks.md) documents this read-only API and clickable references.
2. Edit the board in a `kicad_pcb.edit` block (or, as a fallback, the native file). Keep net assignments,
   layer stack, track widths, clearances and custom rules consistent with the chosen fab and electrical
   requirements. Refill changed copper zones with KiCad (`b.refill_zones()` in the block) before relying
   on their saved fill.

## Check each change

Check the saved board after every step, from the same revision you will hand over:

| The change | Check it with |
| --- | --- |
| The schematic | `cad kicad_sch erc board.kicad_sch` (KiCad's ERC: errors fail it) and `cad kicad_sch snapshot board.kicad_sch tmp/sheet.png --sheet /Power/` for each sheet changed ([schematic](references/schematic.md)) |
| Board against schematic | the pin-by-pin comparison in [schematic](references/schematic.md#into-the-board-and-back): every pad on its schematic pin's net |
| Anything: parts, copper, zones, rules | `cad kicad_pcb drc board.kicad_pcb` (or `--json`): KiCad's DRC against the board's own rules (its `.kicad_pro`'s; without one, KiCad's defaults, which it warns about as `no_project`). It exits 1 on error-severity violations or unconnected items. Unconnected items are the routing still to do |
| Placement | `cad kicad_pcb snapshot board.kicad_pcb tmp/placement.png --display placement`: short, uncrossed ratsnest lines mean a group is placed well; measure decoupling distance and connector access with `kicad_pcb.read` |
| Routing | The layout's property script ([layout](references/layout.md#a-property-check)): segments off 45 degrees, detours, width for current |
| How copper and silkscreen look | `cad kicad_pcb snapshot board.kicad_pcb tmp/copper.png --display copper` (and `--display '{"mode":"copper","side":"bottom"}'`) |
| Ready to order | The review below |

- Review warnings too: KiCad's silkscreen, mask and courtyard rules are warnings, and they are what a
  fab's CAM engineer flags.
- Resolve the cause instead of weakening rules to obtain a clean report.
- A clean DRC establishes the board's own rules, nothing more: not the circuit's correctness and not
  the fab's limits. A number is never read off a snapshot.

## Before ordering

A review of one board, for the fab and assembler it will be ordered from, is a guided review, not a
fab's own engineering check: report what was not checked. Gather evidence in this order: KiCad's DRC
(every error blocks ordering); then measurements DRC cannot make, from the board read back with
`kicad_pcb.read` and the project BOM; then the checklist of what no command measures, with a snapshot.

| Area | Reference | Measured by |
| --- | --- | --- |
| Fabrication | [review-fabrication](references/review-fabrication.md) | KiCad's DRC against the board's rules; the rest by inspection |
| Electrical | [review-electrical](references/review-electrical.md) | the board read back: decoupling distances, narrowest track per net |
| Assembly and sourcing | [review-assembly](references/review-assembly.md) | the part list and placement file, by inspection |

Each finding names its parts by board reference (`U2`, `C8`, `#net:VBUS`); `kicad_pcb.read(path).resolve(ref)`
says where one is.

### Choosing the rules

1. Use the selected fab's own capability page for the board's layer count, copper weight and finish.
   The project's Board Setup and custom rules may differ from the fab's limits: compare them.
2. Where the person names no fab, review against JLCPCB's standard service and say so.
3. Record the source, its date and the conditions (layers, copper, finish) with every limit you
   adopt. If it cannot be checked, report the missing rule rather than invent one.

A fab's standard tier is a price, not a physical limit: finer work is often possible at a surcharge.
Say which it is.

### The review

Scope first: board file and revision, fab and service, layers, copper, finish, assembled or bare.
Then the findings, errors first, each with where (board references), the evidence (the command or
measurement), the rule and its source, the result and the fix; then the coverage: checks run, and
checks not run with what they need. No findings is not a manufacturability approval.

| Item | Evidence | Rule | Result | Fix |
| --- | --- | --- | --- | --- |
| `U2` pad 3 to `C8` | measured 3.67 mm centre to centre from the board read back | decoupling within 3 mm (this review's guide) | review | move `C8` beside pin 3 |

**pass** for a measured item within a cited limit; **fail** for a measured violation or a KiCad
error; **review** for a risk a person decides; **unverified** where evidence or the fab's rule is
missing. Keep cost suggestions (basic vs extended parts, a cheaper finish) apart from manufacturing
constraints. A review alone does not ask for edits or an order: fix only when asked, then check the
neighbours of every fix (a moved capacitor can open a clearance elsewhere). Never order on the
person's behalf.

Export only the requested deliverables from the saved revision you checked; see
[manufacturing and STEP](references/manufacturing.md). A DRC or ERC error blocks writing fabrication
files (Gerbers, drill, placement, BOM, ODB++, IPC-2581) unless the person explicitly says to go ahead;
the report then names every error they went ahead with.

## Show the model

Show the person each model you create or change, and any model or file they ask to see. If your
tools include `cad_show` (your host may prefix it), call it with the model's id or the file's
absolute path; its description says the rest. Otherwise give the person the page's link once: a
model's page is the `view:` line its run prints, and a file's is the `url` that
`cad viewer --json FILE [FILE ...]` prints for it (never guess the port). A file you export is a
download: give its path. Never screenshot the viewer to check your own work; review with
`cad <type> snapshot`. If it fails to launch, say so.

## Board views

The board view supports layers, selection, Measure, annotations and Quick Edit, in 2D and in 3D.
Select works as KiCad's: a click picks a part, pad, track, via, zone, rule area, text, dimension or
graphic, as its Selection Filter ticks them (locked items only when the person ticks them), and a
drag names an area, a box on the layer the person works on. The panel at the left (⌘\ or Ctrl+\
hides and shows it, / searches it) has one search over three tabs. **Parts** lists the parts in the
schematic blocks their footprints record (by kind on a board that records none): a block picks every
part in it. **Nets** lists the nets: a net picks the whole net. Each arrives as a reference
([checks](references/checks.md#references) says what each names and how to resolve it). **Layers**
lists the layers: each layer's eye, and a press for the active layer (drawn on top); under them, how
the board is drawn: Other layers (KiCad's high-contrast modes: the layers but the active one
**Shown**, **Dimmed** or **Hidden**, Ctrl+H cycling them; the outline, and the drills and vias
through an active copper layer, always stay at full strength), the copper pours and the zones' and
tracks' opacity; last, **3D models**, how many parts stand on a model in 3D, with its eye. Under the
tabs, the picked part's or net's pads. The tool strip ends, after its rule, with **Flip** (the side
seen: the board as two stacked layers, the side facing you solid; ⇧F), **2D/3D** (reading **2D** while the
board is flat, **3D** in 3D) and **Display** (the preset: the mode); the zoom is the pill at the
bottom-right. Flip's and 2D/3D's icons are what is on screen and their tooltips what a press does. These are the display, so a Quick Edit's packet
draws the same. The board follows the app's theme: KiCad's colours on the dark canvas, and on the
light one the same colours darkened enough to read (copper stays KiCad's red and blue).

In 3D (**2D/3D**, or the key 3) the board is a slab whose two faces are drawn as the 2D view draws
them, each part standing its 3D model. A press picks what the 2D view picks where the pointer's ray
meets the face, or the part whose body is in front of it; a drag turns the view; **Flip** (or ⇧F)
turns the camera over, and its icon shows the side the camera is on. A part's model is the STEP its footprint names, looked for only in the
board's folder (`${KIPRJMOD}`), KiCad's installed 3D library (every `${KICADn_3DMODEL_DIR}`) and the
folders `CAD_KICAD_3DMODELS` names (separated as `PATH` is); a `.wrl` name is read as the `.step` or
`.stp` beside it. `CAD_KICAD_3DMODELS` is read from the server's environment: a server already
running does not see a variable set in a shell afterwards, so set it before the server starts
(`cad stop`, then run any `cad` command with it set). A part without a model stands as a block, and
**Parts** lists it under **No 3D model**, with why: VRML only (no STEP beside the VRML), not found,
outside the folders above, too large, not a STEP, embedded in the board, or too many models.
`cad kicad_pcb inspect board.kicad_pcb --json` reports each model the same way (`models`: found,
missing with the reason, and the parts that name none), and a STEP or GLB export (`cad kicad_pcb export
--to step|glb`, `kicad_pcb.export`) holds exactly the models found, a `CAD_KICAD_3DMODELS` read from
the command's environment. `cad run kicad-cli` reads KiCad's library as KiCad does: every
`${KICADn_3DMODEL_DIR}` is the first of those library folders, and a `.wrl` name needs its `.wrl` file
there (KiCad 10's library ships STEP alone), so prefer the typed export.

Snapshots use `cad kicad_pcb snapshot`, including `--job` packets saved by Quick Edit. Display modes
are `board`, `copper`, `assembly`, and `placement`. A still is always light (the light canvas and its
colours), whatever the viewer's theme, as every snapshot is:

```bash
cad kicad_pcb snapshot board.kicad_pcb tmp/copper.png --display copper
cad kicad_pcb snapshot board.kicad_pcb tmp/bottom.png --display '{"mode":"copper","side":"bottom","poured":false}'
cad kicad_pcb snapshot board.kicad_pcb tmp/front.png --display '{"layers":["F.Cu","Edge.Cuts"]}'
cad kicad_pcb snapshot board.kicad_pcb tmp/inner.png --display '{"active":"In1.Cu","others":"dimmed","zones":0.3}'
cad kicad_pcb snapshot board.kicad_pcb tmp/front-only.png --display '{"active":"F.Cu","others":"hidden"}'
```

Bottom views mirror the board and its annotations. Native 2D snapshots support the board's plan
camera, layer visibility and saved ink; they do not support 3D Preview, pose or transparency.
The viewer and snapshots draw the board as KiCad's PCB editor shows it (front copper active, pours
at 60%, pad numbers and net names on pads, vias and tracks, dimensions; no drawing sheet, the board alone); they approximate mask/paste openings
and use stroke lettering; text boxes, tables and embedded images are not drawn. KiCad's DRC and manufacturing
exports remain authoritative for fabrication. For an enclosure use KiCad's STEP export, not a
solid inferred from the 2D plot.

## Schematic views

`cad viewer --json board.kicad_sch` opens a schematic a sheet at a time, with the board view's
selection, Measure, annotations and Quick Edit, and its panel: one search over **Parts**, **Nets**
and, for more than one sheet, the **Hierarchy**. The Hierarchy is KiCad's
Hierarchy Navigator: a press shows that sheet. A double-click on a sheet symbol enters it, and the
Hierarchy goes back up; a sheet shown again is where it was left. Select works as KiCad's: a click picks a symbol, pin, wire, label, sheet,
junction or no-connect, as its Selection Filter ticks them, and a drag picks what lies inside the box.
**Parts** lists the parts by the sheet they are placed on, each with its pins, and **Nets** the nets
with the pins on them. A net picked there lights across the sheet shown, and a part on another sheet shows
that sheet. Each arrives as a schematic reference (`#R1`, `#R1.2`, `#net:/MID`, `#sheet:/Power/`,
`#wire:<uuid>`; [schematic](references/schematic.md) says what each names). The schematic follows the
app's theme: KiCad's paper and ink in light, a dark sheet with light ink of the same hues in dark. No
drawing sheet or title block is drawn. ERC findings are not drawn: run `cad kicad_sch erc`. The file
menu's Export offers KiCad's PDF, SVGs, netlist and BOM. Snapshots use `cad kicad_sch snapshot`, and
a Quick Edit packet carries the sheet the view showed. A still is always on KiCad's light paper,
whatever the viewer's theme:

```bash
cad kicad_sch snapshot board.kicad_sch tmp/power.png --display '{"sheet":"/Power/","border":true}'
```