diff --git a/log.md b/log.md index 2343d9e..5a4ffae 100644 --- a/log.md +++ b/log.md @@ -4,6 +4,50 @@ --- +## 2026-04-28 23:55 KiCad 导出修真实连接错：wire_dangling -88%, pin_not_connected -52% + +**Claude 会话** + +接 `fb577cc` 后续。Handoff 选项 #1：用 ERC violation 数从 850 降到接近 0 作为目标。Bisect 出两个根因，都是结构性的 KiCad 语义错（不是浮点 / 精度问题，所以 grid round 不是答案）： + +### Bug A — sym_writer 漏 Y-flip +KiCad lib symbol 是 Y-up，schematic 是 Y-down，placement 时 KiCad 会再翻一次 Y。我们把 EPRO2 (Y-down) 的 PIN/RECT/POLY/CIRCLE/TEXT 坐标直接当 lib coord 写，KiCad 的翻转就把整个 symbol body 上下镜像了。U8 4-pin 磁吸座实测：pin 1↔4 对调、2↔3 对调，结果 wire 端点跟错位的 pin tip 撞不上 → ERC 报 pin_not_connected + wire_dangling。修法：`lib_y = -epro2_y`，pin/text rotation 也镜像 `lib_rot = (360 - rot) % 360`。 + +### Bug B — 没发 net label，KiCad 看不出 EPRO2 的命名网络 +EPRO2 的 WIRE op 带 NET attr（`TXD` / `GND` / `VBUS` ……），多段 LINE 通过同名 NET 连成一个网，**不需要几何相邻**。KiCad 不知道这套，只看几何。修法：在 sch_writer 里查每条 LINE 的 `lineGroup → WIRE → NET attr`，命中就在 LINE 起点 emit 一个 `(label "")`。同名 label 在多条物理 wire 上 → KiCad ERC 才认这是同一个网。**per-LINE 不是 per-WIRE**：单个 WIRE id 下面的 LINE 段不一定共端点，每段都得有 label 才不被判 dangling。 + +### ESP-VoCat 9 sheets ERC 对比 + +| Type | baseline | after | Δ | +|---|---:|---:|---:| +| wire_dangling | 444 | 52 | **−88%** | +| pin_not_connected | 406 | 196 | **−52%** | +| **real connectivity 合计** | **850** | **248** | **−71%** | +| label_dangling | 0 | 111 | new (warn) | +| pin_not_driven | 0 | 23 | new (connector pin 类型问题) | +| endpoint_off_grid | 1372 | 1372 | unchanged (cosmetic, EPRO2 用 30/20/10 mil pitch，不在 KiCad 50 mil 网格上；不能 round——会把 < 50 mil 的 pin 间距压到一起) | +| lib_symbol_issues | 571 | 571 | unchanged (没注册 facere lib，cosmetic) | + +剩余 248 real-connectivity 错主要是 single-sheet ERC 的天然限制：很多网只在一个 sheet 上有这一个 pin，对端在别的 sheet。kicad-cli 一次只看一个 .kicad_sch，看不见跨 sheet。彻底修要 Phase 3（hierarchical 顶层 + sheet links）。 + +### 关键决策（记 Why） + +- **不 round to grid**：50 mil grid 会塌缩 < 50 mil pin pitch（实测 4-pin 磁吸座是 10 mil pitch），破坏几何。EPRO2 源已经在整数 mil，浮点不是 root cause。 +- **per-LINE label 不是 per-WIRE**：同 WIRE id 下两条 LINE 段不共端点是常态（不同地方各连一段），都得 label 才不孤立。 +- **用 `(label)` 不是 `(global_label)`**：实验过两种语法，single-sheet ERC 都判 dangling（因为这个 sheet 上只出现一次）；语义上 EPRO2 net 全局，但 single-sheet 校验视角看不见跨 sheet，换 global_label 帮不上。Phase 3 hierarchical 重构时再切。 +- **不做 ERC config tweak**：KiCad 8 的 connection grid 是硬编码 50 mil，schematic 文件里没法配；想消 endpoint_off_grid 必须破坏 EPRO2 几何或者升级到 KiCad 9 + custom severity。 + +### 测试 + +41 → 46 单测全过：新增 `test_pin_y_negated_for_kicad_lib_y_up_convention` / `test_pin_rotation_mirrored_to_compensate_y_flip` / `test_rect_y_negated` / `test_named_wire_emits_label_at_line_start` / `test_unnamed_wire_emits_no_label`。 + +### 下一步建议 + +- Phase 3 hierarchical：写 root .kicad_sch 引用所有子 sheet + 把跨 sheet 的 NET 升级成 `(global_label)`，single-sheet ERC 残留的 248 + 111 大概率随之降到 < 100。 +- (并行) 消 lib_symbol_issues 571：emit `sym-lib-table` + 独立 .kicad_sym。 + +--- + ## 2026-04-28 23:30 oshwhub 全量 listing 索引落本地：33,695 项 / 28.4 MB **Claude 会话** diff --git a/tools/epro2/kicad/__main__.py b/tools/epro2/kicad/__main__.py index 6d477a3..59d9fbe 100644 --- a/tools/epro2/kicad/__main__.py +++ b/tools/epro2/kicad/__main__.py @@ -51,7 +51,7 @@ def _convert_one( if stats: print( f" {out_path.name}: wires={stats.wires} symbols={stats.symbol_placements} " - f"text={stats.text} skipped={stats.skipped} " + f"text={stats.text} labels={stats.labels} skipped={stats.skipped} " f"lib_emb={stats.lib_symbols_embedded} lib_miss={stats.lib_symbols_missing}" ) return out_path diff --git a/tools/epro2/kicad/sch_writer.py b/tools/epro2/kicad/sch_writer.py index 40f69eb..b6d7d45 100644 --- a/tools/epro2/kicad/sch_writer.py +++ b/tools/epro2/kicad/sch_writer.py @@ -41,6 +41,7 @@ class WriteStats: junctions: int = 0 symbol_placements: int = 0 text: int = 0 + labels: int = 0 skipped: int = 0 lib_symbols_embedded: int = 0 lib_symbols_missing: int = 0 @@ -92,6 +93,14 @@ def write_sch_page( elements: list = [] # 1. Wires from LINE primitives. Each LINE contributes one (wire ...). + # EPRO2 binds wires into nets by NAME (WIRE.NET attr), not just geometry, + # so we also emit a (label "") at one endpoint of each named LINE. + # Same-named labels on physically distinct LINEs are how KiCad's ERC + # recognizes a multi-segment net — without them every LINE looks like a + # dangling stub. We label per-LINE (not per-WIRE id) because a single + # WIRE op may contain segments that don't share endpoints, and KiCad + # flags any unlabeled segment in such a group as wire_dangling. + wire_net_cache: dict[str, str | None] = {} for oid, obj in doc.objects.items(): if obj.get("_type") != "LINE": continue @@ -111,6 +120,24 @@ def write_sch_page( ]) stats.wires += 1 + wire_id = obj.get("lineGroup") + if not wire_id: + continue + wid = str(wire_id) + if wid not in wire_net_cache: + wire_net_cache[wid] = (rel.attrs_dict(wid) or {}).get("NET") + net = wire_net_cache[wid] + if not net: + continue + elements.append([ + Sym("label"), str(net), + [Sym("at"), x1, y1, 0], + [Sym("effects"), [Sym("font"), [Sym("size"), 1.27, 1.27]], + [Sym("justify"), Sym("left"), Sym("bottom")]], + [Sym("uuid"), _new_uuid()], + ]) + stats.labels += 1 + # 2. Symbol placements from COMPONENT ops. Body deferred to Phase 2 (lib_symbols). # For now we emit (symbol ...) entries that reference a placeholder lib_id. # KiCad will draw a red ? but the position + properties are correct. diff --git a/tools/epro2/kicad/sym_writer.py b/tools/epro2/kicad/sym_writer.py index b5c44fc..da6c10a 100644 --- a/tools/epro2/kicad/sym_writer.py +++ b/tools/epro2/kicad/sym_writer.py @@ -16,12 +16,15 @@ Coverage / fidelity: (best-effort; mostly ignored at body level) Coordinate convention: - EPRO2 SYMBOL primitives use **mil** (same as schematic); we convert via - ``MIL_TO_MM = 0.0254``. KiCad lib symbol coords are **Y-up** internally, - but the placement of pins relative to body origin is what matters; for - ESP-VoCat the empirical Y orientation is consistent (pins on left at -X, - pins on right at +X), so we do not flip Y. If KiCad renders flipped, the - fix is a per-axis sign in ``_pt`` here. + EPRO2 SYMBOL primitives use **mil** in a Y-down frame (same as the + schematic). KiCad lib symbol coords are **Y-up**; when a symbol is + placed on a (Y-down) schematic KiCad re-flips the lib's Y. To make the + rendered placement land at the EPRO2 absolute position (so wire endpoints + meet pin tips) we therefore **negate Y in lib coords**, and mirror pin / + text rotations across the X-axis (``rot_lib = -rot_epro2 mod 360``). + Without this, vertically-arranged pins end up at Y-mirrored positions — + ERC then reports ``pin_not_connected`` even when the wire endpoint and + pin tip share the same X. """ from __future__ import annotations @@ -60,6 +63,20 @@ def _pt(v) -> float: return 0.0 +def _y(v) -> float: + """Y for lib symbol space: negate (Y-down EPRO2 → Y-up KiCad lib).""" + return -_pt(v) + + +def _lib_rot(rot) -> float: + """Mirror pin/text rotation across the X-axis to compensate for the lib + Y-up vs schematic Y-down flip KiCad applies on placement.""" + try: + return (360.0 - float(rot or 0)) % 360.0 + except (TypeError, ValueError): + return 0.0 + + def _stroke(width: float = 0.254) -> list: return [Sym("stroke"), [Sym("width"), width], [Sym("type"), Sym("default")]] @@ -110,8 +127,10 @@ def write_lib_symbol(doc: Document, *, lib_prefix: str = "facere") -> list | Non if obj.get("partId") != part_id: continue if t == "RECT": - x1, y1 = _pt(obj.get("dotX1")), _pt(obj.get("dotY1")) - x2, y2 = _pt(obj.get("dotX2")), _pt(obj.get("dotY2")) + # KiCad lib uses Y-up; we negate Y so the rectangle stays oriented + # the same way it appears in EPRO2 after placement Y-flip. + x1, y1 = _pt(obj.get("dotX1")), _y(obj.get("dotY1")) + x2, y2 = _pt(obj.get("dotX2")), _y(obj.get("dotY2")) body.append([ Sym("rectangle"), [Sym("start"), x1, y1], @@ -122,7 +141,7 @@ def write_lib_symbol(doc: Document, *, lib_prefix: str = "facere") -> list | Non elif t == "POLY": pts = obj.get("points") or [] xy_list = [Sym("pts")] + [ - [Sym("xy"), _pt(p.get("x")), _pt(p.get("y"))] for p in pts + [Sym("xy"), _pt(p.get("x")), _y(p.get("y"))] for p in pts if isinstance(p, dict) ] if len(xy_list) >= 3: # at least 2 points + the "pts" tag @@ -135,7 +154,7 @@ def write_lib_symbol(doc: Document, *, lib_prefix: str = "facere") -> list | Non elif t == "CIRCLE": body.append([ Sym("circle"), - [Sym("center"), _pt(obj.get("centerX")), _pt(obj.get("centerY"))], + [Sym("center"), _pt(obj.get("centerX")), _y(obj.get("centerY"))], [Sym("radius"), _pt(obj.get("radius"))], _stroke(), _fill(), @@ -146,8 +165,8 @@ def write_lib_symbol(doc: Document, *, lib_prefix: str = "facere") -> list | Non continue body.append([ Sym("text"), val, - [Sym("at"), _pt(obj.get("x")), _pt(obj.get("y")), - float(obj.get("rotation") or 0)], + [Sym("at"), _pt(obj.get("x")), _y(obj.get("y")), + _lib_rot(obj.get("rotation"))], _font(), ]) elif t == "PIN": @@ -158,8 +177,8 @@ def write_lib_symbol(doc: Document, *, lib_prefix: str = "facere") -> list | Non elec = PIN_TYPE_MAP.get(pin_type_raw, "passive") body.append([ Sym("pin"), Sym(elec), Sym("line"), - [Sym("at"), _pt(obj.get("x")), _pt(obj.get("y")), - float(obj.get("rotation") or 0)], + [Sym("at"), _pt(obj.get("x")), _y(obj.get("y")), + _lib_rot(obj.get("rotation"))], [Sym("length"), _pt(obj.get("length"))], [Sym("name"), pin_name or "~", _font()], [Sym("number"), pin_number or "~", _font()], diff --git a/tools/epro2/tests/test_sch_writer.py b/tools/epro2/tests/test_sch_writer.py index 4d4ca57..fce4020 100644 --- a/tools/epro2/tests/test_sch_writer.py +++ b/tools/epro2/tests/test_sch_writer.py @@ -100,6 +100,46 @@ def test_text_object_emits_text_block_when_non_empty(): assert texts[0][1] == "Hello" +def test_named_wire_emits_label_at_line_start(): + """EPRO2 binds wire segments into nets by NAME (WIRE.NET attr), not by + geometry alone. Each LINE whose lineGroup points to a WIRE with a NET + attr must get a (label "") at one endpoint — same-named labels on + distinct LINEs are how KiCad's ERC recognizes a multi-segment net.""" + d = _doc([ + ("w1", {"_type": "WIRE"}), + ("a1", {"_type": "ATTR", "parentId": "w1", "key": "NET", "value": "GND"}), + ("ln1", {"_type": "LINE", "lineGroup": "w1", + "startX": 100, "startY": 0, "endX": 200, "endY": 0}), + ("ln2", {"_type": "LINE", "lineGroup": "w1", + "startX": 300, "startY": 0, "endX": 400, "endY": 0}), + ]) + text = write_sch_page(d, sheet_origin_mm=(0.0, 0.0)) + p = parse(text) + labels = _block(p, "label") + assert len(labels) == 2 # one label per non-degenerate LINE + assert all(lab[1] == "GND" for lab in labels) + # First label sits at the first LINE's start endpoint + at = next(c for c in labels[0] if isinstance(c, list) and c[0] == "at") + assert at[1] == 100 * MIL_TO_MM + assert at[2] == 0.0 + assert getattr(write_sch_page, "last_stats").labels == 2 + + +def test_unnamed_wire_emits_no_label(): + """A WIRE without a NET attr (or a LINE without a lineGroup) gets no + label — emitting a label without a name would be syntactically invalid + and semantically meaningless.""" + d = _doc([ + ("w1", {"_type": "WIRE"}), # no NET attr + ("ln1", {"_type": "LINE", "lineGroup": "w1", + "startX": 0, "startY": 0, "endX": 100, "endY": 0}), + ]) + text = write_sch_page(d, sheet_origin_mm=(0.0, 0.0)) + p = parse(text) + assert _block(p, "label") == [] + assert getattr(write_sch_page, "last_stats").labels == 0 + + def test_non_sch_page_doc_rejected(): d = Document(doc_uuid="x", doc_type="PCB") try: diff --git a/tools/epro2/tests/test_sym_writer.py b/tools/epro2/tests/test_sym_writer.py index 7576dfb..d9a451e 100644 --- a/tools/epro2/tests/test_sym_writer.py +++ b/tools/epro2/tests/test_sym_writer.py @@ -127,6 +127,58 @@ def test_sch_writer_embeds_lib_symbols_via_project_relations(): assert stats.lib_symbols_missing == 1 +def test_pin_y_negated_for_kicad_lib_y_up_convention(): + """KiCad lib uses Y-up; the schematic uses Y-down and KiCad re-flips Y on + placement. To make the rendered placement land where EPRO2's wire ends + expect it, sym_writer must NEGATE Y for lib coords. Without this, + vertically arranged pins land at Y-mirrored positions and ERC reports + pin_not_connected even when wire and pin share an X coord.""" + d = _sym_doc("sym1", "MyPart.1", [ + ("e5", {"_type": "PIN", "partId": "MyPart.1", + "x": -20, "y": 10, "length": 20, "rotation": 0}), + ]) + entry = write_lib_symbol(d) + parsed = parse(to_sexpr(entry)) + inner = next(c for c in parsed if isinstance(c, list) and c[0] == "symbol") + pin = next(c for c in inner if isinstance(c, list) and c[0] == "pin") + at = next(c for c in pin if isinstance(c, list) and c[0] == "at") + # EPRO2 y=10 → lib y=-10 mil = -0.254 mm + assert at[1] == -20 * 0.0254 + assert at[2] == -10 * 0.0254 + + +def test_pin_rotation_mirrored_to_compensate_y_flip(): + """Pin angle in lib must mirror across X-axis (rot' = 360-rot mod 360) + so that after KiCad's lib→sch Y-flip the pin extends in the same + direction it does in EPRO2.""" + d = _sym_doc("sym1", "MyPart.1", [ + ("e5", {"_type": "PIN", "partId": "MyPart.1", + "x": 0, "y": 0, "length": 10, "rotation": 90}), + ]) + entry = write_lib_symbol(d) + parsed = parse(to_sexpr(entry)) + inner = next(c for c in parsed if isinstance(c, list) and c[0] == "symbol") + pin = next(c for c in inner if isinstance(c, list) and c[0] == "pin") + at = next(c for c in pin if isinstance(c, list) and c[0] == "at") + assert at[3] == 270.0 # 90 → 270 + + +def test_rect_y_negated(): + d = _sym_doc("sym1", "MyPart.1", [ + ("r1", {"_type": "RECT", "partId": "MyPart.1", + "dotX1": -10, "dotY1": -5, "dotX2": 10, "dotY2": 5}), + ]) + entry = write_lib_symbol(d) + parsed = parse(to_sexpr(entry)) + inner = next(c for c in parsed if isinstance(c, list) and c[0] == "symbol") + rect = next(c for c in inner if isinstance(c, list) and c[0] == "rectangle") + start = next(c for c in rect if isinstance(c, list) and c[0] == "start") + end = next(c for c in rect if isinstance(c, list) and c[0] == "end") + # Y inputs were -5 and 5 → after negation: 5 and -5 + assert start[2] == 5 * 0.0254 + assert end[2] == -5 * 0.0254 + + def test_sch_writer_without_project_relations_emits_empty_lib_symbols(): sch = Document(doc_uuid="sch1", doc_type="SCH_PAGE") sch.objects["e1"] = {"_type": "COMPONENT", "partId": "X.1", "x": 0, "y": 0}