EasyEDA Schematic

EasyEDA schematic automation skill. Use when working with EasyEDA schematic pages through the easyeda-agent CLI or daemon, including reading schematic context, listing components, placing or modifying components, creating wires and net flags, selecting primitives, running schematic DRC, saving schematic changes, and exporting BOM or netlist artifacts.

Use easyeda-agent typed actions. Do not write raw EasyEDA JavaScript unless a typed action is missing and the user explicitly accepts a debug path.

Workflow

1. Run easyeda health.
2. Read active project and schematic context.
3. Inspect before mutating.
4. Prefer small additive operations.
5. Verify each mutation by readback, snapshot, or DRC.
6. Ask before destructive operations, multi-step mutation plans, or saving.
7. Summarize changed primitives, warnings, and artifacts.
8. If an official EasyEDA API is missing, undocumented, or differs from runtime behavior, record the evidence and workaround; when it affects correctness or maintainability, prepare a minimal repro and file an issue with the relevant official EasyEDA repository.

Production preflight gates

• Sheet first, default A4. Before any whole-board placement/routing, run easyeda doc ls, switch to the target schematic page, then run easyeda sch sheet-geometry --json. If no componentType:"sheet" bbox is available, stop and ask the user to select/create the default A4 sheet in EasyEDA; do not place parts, wire nets, or run sch autolayout --apply on a sheetless page.
• Page plan before coordinates. For non-trivial designs, decide the page/module split from the A4 usable area before placing anything. If the modules do not fit with route channels and title-block keep-out, create/rename pages and split modules instead of expanding coordinates outside the sheet.
• Clear is destructive. Use easyeda sch clear --dry-run first, report the delete counts, and wait for explicit confirmation before easyeda sch clear. Preserve the sheet by default; only use --no-preserve-sheet when the user explicitly wants the drawing frame removed too. After clearing, read back the page and confirm only the intended sheet/template primitives remain.
• Honor step confirmations. If the user asks to confirm each step, stop after every stage report (preflight, clear dry-run, clear apply, page creation, placement dry-run, placement apply, wiring, verification, save) until they approve the next mutation.

Drawing a schematic — library-first (default)

Design conventions live in the sibling easyeda-conventions skill (layout zones, spacing, wire/orientation rules, part-selection criteria, the canonical orientation table + standard-parts library). This operational skill links to it — single source, never copy the rules here.

⚠️ 整板 / 非平凡设计 → 先走 easyeda-design-flow 流程脊柱。 那里有分阶段 + 硬门禁(预分析 → 分页 → 模块编组 → 按组摆放 → 通道布线 → DRC + layout-lint → 调整闭环), 专治「随手摆导致覆盖、外围乱飞、线压元件」。本 skill 提供它每一步要调用的具体动作。

⚠️ 多器件 / 整板设计:先花几分钟摸底,再动手。 非平凡板子(>~10 件,或要交付/排 PCB) place 前快速读懂设计(器件/电源树/功能分组/幅面)——见 design-pre-analysis.md(轻量摸底,不是门禁)。 然后照 auto-layout-sop.md 的 CLI 能力 + 硬坑落坐标,布局用数据 + 截图自调(放→读回坐标→sch layout-lint 判覆盖/间距→挪→再验)。 小改 / 几个器件直接按下面放置。

Place real parts from the EasyEDA / 立创(LCSC) library, then wire them. Hand-drawing a custom component symbol is the fallback, used only when the part genuinely isn't in the library (a hand-built symbol loses the footprint/supplier linkage and is error-prone — prefer a library part, even a near-equivalent, first).

0. Standard parts first. Check standard-parts.json (in the easyeda-conventions skill) for the category you need (10k 0402, 100nF, ESP32-S3, AMS1117, USB-C, …). If it's there, place straight from its { libraryUuid, deviceUuid } — deterministic, BOM-ready, with the real LCSC C-number. Only search when the category is missing, and ADD the chosen part back to standard-parts.json (with its C-number) so the next design is reproducible. When you already know the exact C-number (from a BOM or standard-parts.json), resolve it deterministically with lib by-lcsc --lcsc C… (schematic.library.get_by_lcsc) → {libraryUuid, uuid} ready to place, skipping free-text ranking. After a new selection, scripts/parts-add.py appends the resolved part into standard-parts.json so the curated cache grows (it reads the JSON lib by-lcsc / lib search emits).
1. Search (fallback) schematic.library.search (free-text: an MPN, value+package, or a name like ESP32-S3-WROOM-1). Results are reranked by relevance (best category first; each carries a score), so the right part usually leads — but still sanity-check value/footprintName/lcsc before placing. Each candidate carries uuid, libraryUuid, name, footprintName, lcsc, manufacturerId.
2. Place schematic.component.place with the chosen {libraryUuid, uuid} at a coordinate → a manufacturable part with correct symbol + footprint + LCSC number. ⚠️ --uuid must be a DEVICE-library uuid (from lib search / standard-parts.json), never one of the uuid-looking fields component/symbol/footprint/uniqueId that sch list reports — those are placed-INSTANCE ids and cannot be replayed. Feeding an instance uuid hangs the EasyEDA API; sch place now fails fast (~8s) with a hint instead of stalling 20s on context deadline exceeded. To re-place an existing part, run lib search again to get its device uuid.
3. Read pins (schematic.components.list / pin readback) for exact pin coordinates before wiring.
4. Wire (reference-validated — see 画线 / flag / 去耦(CLI 级硬规则) in auto-layout-sop.md; the 嘉立创 ESP32-S3 standard project is flags only on power/ground rails, every signal a real local wire):
   • Signals = real local orthogonal wires (pin→wire→pin). Endpoint on a pin coord = connected; non-aligned pins → L-route [x1,y1, x2,y1, x2,y2].
   • ⚠️ Never run a wire through another pin — EasyEDA trims+connects it there. Route in pin-free channels.
   • ⚠️ Multi-pin nets: chain pin→pin (each segment anchored on a pin), NOT a star to a free junction (EasyEDA drops the un-anchored junction on merge).
   • Flags ONLY for power/ground rails (connect_pin direction=, never blanket rot 0).
5. Verify with easyeda sch layout-lint(布局:覆盖/间距)+ schematic.drc.check(电气)
   • the data linter (scripts/lint.sh <project>). ⚠️ After API edits the EasyEDA canvas may not auto-redraw → schematic.snapshot / getCurrentRenderedAreaImage return a STALE frame (even view fit framing is stale). Judge STATE by data (sch list/getAll), use the screenshot for visual layout only, and touch the page in EasyEDA (scroll/ click) to force a redraw before trusting a snapshot. schematic.snapshot now returns primitiveCount + capturedAt alongside the artifact — compare primitiveCount across two adjacent snapshots: if it changed but the image bytes/sha did not, the frame is stale and must not be trusted for verification.

Bulk realization from a netlist (automated)

For a whole board (place ~N parts + wire the full netlist at once), the manual flow above doesn't scale. Pipeline (proven on box-v2/110 parts):

1. PLACE-ALL — for each part, resolve {libraryUuid, deviceUuid} (standard-parts.json first, lib.search fallback), place at coords, then assign the designator (sch modify --patch '{"designator":...}' — place leaves it C?).
2. READ-PINS — ONE sch list / pin pull AFTER all placement for real pin coords (don't trust pre-place maps; map IC functional names → physical pads first).
3. WIRE — per net, decide flag vs local wire vs label (see the decision table in the SOP); emit flags via connect_pin direction= (never blanket rot 0).
4. DRC + lint, then a MANDATORY clustering/zone pass before "done".

⚠️ Layout is NOT optional. Naive place-at-synthesis-coords + flag-every-pin is electrically valid but visually scattered (box-v2: 327 flags, decaps far from ICs). Follow auto-layout-sop.md (easyeda-conventions): fit sheet → mains by zone → auxiliaries pin-relative to their owner IC → fine-tune. And write resolved parts back into standard-parts.json in the same change (so the next board doesn't re-search non-deterministically).

Churn-resilience for >~50 mutations (essential, see the SOP): route by --project; batch many primitives per debug.exec_js; chunk each batch to <~20s (long calls die to the heartbeat); heavy-retry + incremental sch save per chunk; re-pull fresh pids each chunk.

Pin-aware autoconnect — let the planner pick direction/offset

connect_pin (sch connect) keeps the connection safe (pin → short wire → flag/netport, never a netflag on a bare pin), but it still makes YOU pick --direction and --offset, so layout quality depends on judgment. sch autoconnect removes that judgment: it pulls the real geometry (part bboxes, pin coords, existing flag/port/label bboxes, title-block keep-out), scores every up/down/left/right × offset candidate with a deterministic cost function (part overlap / title-block / pin-crossing / flag-collision / through-part penalties, shortest-offset + outward-side + kind-default bonuses), picks the lowest-cost one, and delegates the mutation to connect_pin. Same schematic state + spec → same selection (deterministic).

bash

# single pin by designator:pin (number OR name)
easyeda sch autoconnect --pin U1:41 --kind gnd --net GND
easyeda sch autoconnect --pin U1:3V3 --kind power --net +3V3

# explicit coordinates (compat with existing flows)
easyeda sch autoconnect --x 720 --y 670 --kind gnd --net GND

# preview the plan + rejected options WITHOUT mutating
easyeda sch autoconnect --pin U1:41 --kind gnd --net GND --dry-run --json

# batch spec — clustered pins auto-stagger so labels don't stack
easyeda sch autoconnect --spec p1-connect.json

Spec JSON (--spec): {"connections":[{"pin":"U1:41","kind":"gnd","net":"GND"}, {"pin":"U1:3V3","kind":"power","net":"+3V3"}], "rules":{"avoidTitleBlock":true, "avoidPinFanout":true,"staggerLabels":true,"offsetRange":[18,80],"offsetStep":6, "minLabelGap":12}}. Each result reports the selected candidate (direction / offset / endPoint / score), the rejected alternatives with reasons, and the wirePrimitiveId / flagPrimitiveId. The title-block keep-out comes from the shared sch sheet-geometry derivation (issue #26) — when the sheet bbox isn't exposed it is reported as provisional and not geometrically enforced (so a guessed box can't corrupt scoring). Prefer sch autoconnect over hand-picking sch connect --direction/--offset for power/ground/netport stubs; sch connect stays for when you deliberately override the geometry.

Module-aware autolayout — place parts by module zone

Where autoconnect is pin-level, sch autolayout is module-level placement: it reads a --spec (page, sheet, modules with zone/core/parts, rules), pulls the real geometry (anchors + bboxes + core pins + sheet bbox), partitions the usable canvas into named zones (left-top / left-bottom / center / right / right-top / right-bottom / …), places each module's core IC near its zone center, fans the peripherals around the core with collision retry, and keeps each core pin's fanout channel and the A4 title-block clear. Same pure-scorer style as autoconnect: identical spec + input → identical coordinates that pass sch layout-lint.

bash

# preview proposed coordinates + warnings, mutate nothing (default)
easyeda sch autolayout --spec p1-layout.json --dry-run

# move parts via schematic.component.modify, then self-check overlaps
easyeda sch autolayout --spec p1-layout.json --apply

# structured report
easyeda sch autolayout --spec p1-layout.json --json

Spec JSON (--spec):

json

{
  "page": "P1_MCU_USB_STORAGE", "sheet": "A4",
  "modules": [
    {"name":"USB_HUB","zone":"left-top","core":"U10","parts":["J2","U10","X1","C30","R15"]},
    {"name":"MCU","zone":"center","core":"U1","parts":["U1","C18","C19","R6"]},
    {"name":"SD_NAND","zone":"right","core":"U8","parts":["U8","C28","R10"]}
  ],
  "rules": {"avoidTitleBlock":true,"preservePinFanout":true,
            "moduleGap":80,"routeChannelGap":40,
            "preferVerticalPeripheralPlacement":true}
}

The result reports each placement (designator / x / y / rotation / module), any warnings (e.g. a peripheral forced into a fanout lane, or a spec part not yet placed), and a validation summary (partOverlaps / titleBlockHits / fanoutKeepoutHits). Notes:

• v1 moves already-placed parts only — it does NOT create missing parts; a spec part absent from the page is warned + skipped. Place the parts first (library-first), then autolayout arranges them.
• A missing core is a hard error for that module (clear diagnostic).
• When the sheet bbox isn't exposed, the title-block keep-out is reported as provisional and not geometrically enforced.
• autolayout solves module placement, not routing — follow it with sch autoconnect (power/ground/netport) + wiring, then sch layout-lint / sch drc to gate.

Actions

Run easyeda actions for the current machine-readable action list.

导航 / Navigation

自助「发现 + 切换」闭环（首选） — 不要让用户手动开窗口/切页,Agent 自己发现并切换:

bash

easyeda daemon health                         # 发现:有哪些已连接窗口 + 各自实时上下文
easyeda doc ls     --project <名字>            # 发现:列出该窗口所有可开文档(原理图页+PCB),★=当前前台
easyeda doc switch <P2|PCB1|uuid> --project <名字>   # 切换:按页名/PCB名/uuid 切到前台,自动回读确认

• easyeda doc ls 聚合了 schematic.pages.list + pcb.documents.list + document.current,一条命令看全貌;--json 给机器读。
• easyeda doc switch 按名字解析 → document.open → document.current 回读确认。同名页(多个 P1)会报歧义并列出 uuid,改传 uuid。跨类型也行(PCB ↔ 原理图)。
• 多窗口时必须 --project(或 --window):doc ls/doc switch 不带目标时,只有「恰好一个窗口」才能自动命中;两个及以上窗口会报 no EasyEDA connector is available。同理,某窗口连接器正在重连(churn)的瞬间也可能瞬时报这个,重试即可。

底层 action(需要细控时再用):

• project.current — 当前工程信息（uuid / name / teamUuid）
• document.current — 当前激活文档信息（uuid / tabId / documentType）—— 实时读取,不是连接快照
• document.open — 按 UUID 打开任意文档（原理图页或 PCB），通用版切换入口
• schematic.pages.list — 列出工程内所有原理图及页面
• schematic.page.open — 按 UUID 切换到指定原理图页（等同于 document.open，保留兼容）

多窗口说明：EasyEDA 每个窗口对应一个独立的 connector（windowId）。easyeda daemon health 列出所有已连接窗口;优先用 --project <名字> 路由(windowId 重连会变),细控时才用 --window <windowId>。

上下文是实时的,不会卡在 home。 两条刷新路径:① daemon 用每次 action 响应里的实时上下文刷新缓存;② 连接器 v0.5.7 起,心跳(~3s)会主动重读当前文档,变了就推——所以用户在 EasyEDA 里切了 tab、什么命令都没跑,daemon health 也会在 ~3s 内自己跟上。若 health 显示某窗口是 home,说明它的前台 tab 停在开始页/欢迎页,或那个窗口跑的是旧连接器(< v0.5.7)没连上。

UI 切页要双击:单击只选中 tab、不打开文档;双击才真正打开,document.current 读到的是「已打开」的那个文档。

connectorVersionOk: false = 该窗口加载的连接器版本与 daemon 不符(典型:开着的窗口跑着旧连接器代码)。处理:完全退出并重启 EasyEDA 重新加载连接器(re-import 不会刷新已开窗口)。null 表示版本号非 semver(dev 构建)无法判定。

原理图编辑

• schematic.components.list — --include-bbox 附带每个元件渲染范围 {minX,minY,maxX,maxY}(供布局推理);--include-pins 附带每脚 {pinName,pinNumber,x,y,noConnected}(布线/连通性判断的数据面,布线前读引脚功能名→坐标用它,不要再用 easyeda call schematic.components.list --payload '{"includePins":true}' 绕过)。两个 flag 可与 --all-pages 叠加(输出会显著变大)。
• easyeda sch layout-lint — 布局自检(治覆盖的机械真值)。拉 components.list --include-bbox,Go 侧两两几何检查:bbox 重叠 = ERROR(命令非零退出,可当门禁)、间距 < --min-gap(默认 2.54mm)= WARN。--all-pages、--json。默认只检真实器件(componentType == "part"):图框/标题栏(sheet)铺满整页、netflag/netport/netlabel 等非器件原语都会被自动排除,否则它们会与几乎每个器件误报重叠(见 issue #13)。需要把这些也纳入检查时加 --include-non-parts;被排除的数量会在报告里以 skippedNonParts 透明列出。摆放后跑它判覆盖/间距,比肉眼/截图可靠(截图可能 stale)。是 place→verify→adjust 闭环的输入。
• easyeda sch sheet-geometry — 图纸边界 + 标题栏 keep-out(放置/布线规划器的统一几何源,issue #26)。读 components.list --include-bbox 里 componentType == "sheet" 的实测 bbox,按长宽比匹配已知模板(A 系列横/纵向 ≈ √2),在右下角按归一化比例切出标题栏(图框/明细表)子矩形;schematic.titleblock.get 的 showTitleBlock 隐藏时不输出 keep-out。返回 {sheet, titleBlock, keepouts[], warnings[]},每项带 provenance(known-template-ratio / fallback-ratio / none),无法确定时只给 warning、不输出虚假精度。--json。规划器消费 keepouts[]({name,bbox,hard})即可,不要再各处硬编码 A4 坐标。比例表见 easyeda-conventions/references/sheet-templates.json。
• schematic.component.place
• schematic.component.modify
• schematic.component.delete — ⚠️ 只删组件,不删导线/总线/图形。删完 schematic.components.list 只剩 A4 sheet 会让你误以为页面已干净,实际残留导线还在(DRC 仍会报)。要真正清页用 schematic.page.clear。
• schematic.page.clear — 一键清空当前页:删除所有页级 primitive(组件、网络标志/端口/标签、导线、总线、图形),默认保留图框 sheet(--no-preserve-sheet 连图框一起删)。--dry-run 只统计不删。返回各类型删除计数 {deleted:{...}, total, deletedIds}。无 undo,确认门控。生成→检测→清页→重试闭环用这个。生产流程必须先 dry-run、报告、等用户确认;清完再读回确认 sheet 仍在。CLI:easyeda sch clear [--dry-run] [--no-preserve-sheet]。
• schematic.primitives.delete — 按 id 跨类型删除(组件/标志/导线/总线/图形都行),省略 --ids 则删当前选区(配合 schematic.select 做"全选→删除")。无 undo,确认门控。CLI:easyeda sch prim-delete [--ids '[...]']。
• schematic.wire.create
• schematic.netflag.create
• schematic.power.connect_pin
• schematic.pin.set_no_connect — 打/清「非连接标识」(NC, X 标记),让 DRC 不再对故意悬空的引脚报"未连接"。按位号+引脚号定位:easyeda sch no-connect --designator U1 --pin 23,24[,…](--clear 清除)。
• schematic.select
• schematic.snapshot — 截图。产物保存在 CLI 运行目录下的隐藏目录 <cwd>/.easyeda/artifacts/,文件名带本地时间戳(<YYYYMMDD-HHMMSS>-<kind>-<短id>.png,便于排序/查找);响应里的 artifacts[].path 是绝对路径。netlist/BOM 等其他产物同此规则。
• schematic.drc.check — 用 easyeda sch drc 跑 EasyEDA SDK 的 sch_Drc.check。注意:当前 EasyEDA build 可能只返回布尔/聚合结果,不会暴露 UI DRC 面板里的逐条 warning(例如网络标识与导线名不一致、悬空脚明细)。所以它只能作为 SDK DRC 门,不能单独宣称“官方 DRC 干净”。
• schematic.check — 用 easyeda sch check 跑的重建式逐条设计检查(补 SDK DRC 暴露不全):net-marker-mismatch(网络标识/端口/标签名与所连导线 net 名不一致)、multi-net-wire(同一导线多个网络名)、floating-pin(引脚悬空)、wire-crossing(导线交叉)、wire-over-pin(导线穿过引脚)。floating-pin 现在带 primitiveId 与 pinDetails[](每个悬空脚的 number/name/x/y),文本报告逐脚打印脚名+坐标、designator 为空时回退打印 primitiveId,可直接喂给 sch no-connect。wire-over-pin 会排除落在导线端点或 netflag/netport/netlabel 锚点上的引脚——那是 sch connect 短 stub 的合法终点(EasyEDA 把共线相邻 stub 自动合并成一条长导线时,内部引脚会落进合并后导线的内部,但官方 DRC 视为合法,故不再误报)。--json、--strict(有 finding 即非零退出)、--all-pages。
• schematic.save
• schematic.export.netlist
• schematic.export.bom
• schematic.library.search
• schematic.library.get_by_lcsc — 用 easyeda lib by-lcsc --lcsc C…(可重复或逗号分隔多个)把 LCSC C 号确定性解析成 {libraryUuid, uuid}(免 free-text 排序),返回里带 notFound 列出未解析的 C 号。已知确切器件(BOM / standard-parts.json)时优先用它。

PCB

PCB 操作（切到 PCB、读器件/层/网络/Board、从原理图 import_changes 同步、布局摆位 move/rotate/align/distribute/grid_snap/cluster-arrange）在独立的 operational skill easyeda-pcb —— 见那里(单一真源,勿在此复制)。

Bundled Scripts

脚本	用途
scripts/sch.py	稳定执行器（import 用）— 把核心 CLI 封成 churn-resilient API:read()/place()/move()/wire()(SOP-W 正交避引脚)/rail_flag()(SOP-F 定向)/decouple()(SOP-D)/connectivity()(union-find 真连通)/snapshot()(取 .easyeda/artifacts)。AI 数据自调闭环用:放→read→判→move→connectivity 验。
scripts/lint.sh <project>	原理图数据 lint（几何 + 连通性检查，无需截图）。有 baseline 时显示 DIFF
scripts/lint.sh <project> --save	全量 lint 并记录 baseline
scripts/bom-enrich.py <bom.tsv>	将导出的 BOM 里 SupplierId 从 MPN 补全为 LCSC C 号。easyeda bom export --type csv 已默认自动调用它就地补全（--enrich=false 关闭）；本脚本仅在手动后处理已有 BOM 时单独用
scripts/parts-select.py	器件选型辅助工具

标准器件库（standard-parts.json）、flag 旋转真值表（orientation.json）、布局/选型约定都在 easyeda-conventions skill（单一真源，勿在此复制）。 bom-enrich.py / parts-select.py / orient.py 会跨 skill 自动读取这些 canonical 文件。

Guardrails

• Confirm before deleting primitives.
• Confirm before saving unless the user explicitly asked to save.
• 持久化:place/wire/modify 只改 EasyEDA 内存,不 schematic.save 就不落盘 —— 窗口重载 / daemon 重启 / EasyEDA 崩溃会丢掉未保存的改动(实测踩过)。daemon 默认开防抖 autosave(3s) 兜底(daemon start --autosave-debounce,0 关),但防抖窗口内进程挂掉仍会丢最后几笔,所以多步改动仍分批显式 sch save,别只靠 autosave。整板流程的存盘节奏见 easyeda-design-flow 的 💾 检查点。
• Confirm before running a generated multi-step mutation plan.
• Do not claim completion after mutation until verification succeeds or the remaining risk is stated.
• Treat File and Blob outputs as artifacts.
• If DRC fails, report violations and propose the smallest repair step.

Layout Conventions

原理图

When placing components, follow the easyeda-conventions skill — schematic-layout-conventions.md:

• Zone map (power left, MCU center, RF/sensors right, big modules in corners)
• Module spacing rules (80–500 units depending on size + pin count)
• Wire stub lengths (20–40 units for power, 20–60 for signals)
• Right-angle-only routing, decoupling caps within 30 units of VCC pins

PCB 布局约定在 pcb-layout-conventions.md，操作流程在 easyeda-pcb skill。

EasyEDA Electrical Rules (load-bearing — DRC will fatal if ignored)

EasyEDA's DRC does not treat two primitives sharing the same coordinate as electrically connected. Every connection needs a real schematic.wire.create between them. Two concrete consequences:

1. schematic.netflag.create MUST NOT be placed on the same point as a pin. Placing a +3V3/GND/IN/OUT flag at the exact pin coordinate produces a DRC fatal: "端点重叠且未连接 / endpoints overlap but not connected". The flag sits on top of the pin visually but EasyEDA treats them as two disjoint endpoints.

   Correct pattern: pin → short wire → netflag at the wire's far end. Typical offset: 20 grid units (EasyEDA uses 0.01 inch / grid unit on schematics). Example for +3V3 on R1.pin1 @(265, 440):

   text

   schematic.wire.create     points = [265,440, 245,440]   # pin to a free point
   schematic.netflag.create  x = 245, y = 440, kind=power, net="+3V3"
   

2. Wires must have non-zero length. A wire of [x,y, x,y] is silently ignored; a wire of [x,y, x+0,y+0] will not register a connection.

3. NC pins still need explicit marking. A pin without any wire/flag triggers a "悬空 / floating" warning even if your design intends it unused. Use a Non-Connected flag for those.

Apply this rule when generating any power/ground/port connection — emit the wire first, then place the flag at the wire's free endpoint.

Missing Actions

When a needed operation has no typed action:

0. Discover the underlying eda.* method first — easyeda api search <kw> (offline, no daemon) ranks methods of the official API by name/namespace/中文摘要, easyeda api ls [filter] lists namespaces, easyeda api show <ns> dumps one namespace. Index is embedded from @jlceda/pro-api-types. This is the front of the dev loop api search → debug.exec_js → typed action → Cobra 子命令.
1. Decompose it into existing actions if possible.
2. Otherwise state the missing action name and expected inputs/outputs.
3. Use debug.exec_js (raw eda.* JavaScript) only as a temporary, user-confirmed debug escape hatch. Its result must be JSON-serializable — base64-encode any Blob/File inside the snippet.
4. Recommend promoting repeated debug code into a typed action.