Inne · Budowanie i kod
schematic-design
/schematic-design
Wykonuje plan rozmieszczenia elementów na schemacie elektronicznym i wprowadza zmiany w istniejącym schemacie.
- Autor
- productofamerica ↗
- Repozytorium
- mcp-server-kicad ↗
- Licencja
- GPL-3.0
- Ostatnia zmiana repozytorium
- 23.10.2026
Ocena i bezpieczeństwo
100/ 100Klasa: dobry
Format25 / 25
Frontmatter z nazwą i opisem, poprawna nazwa, opis do 1024 znaków, nazwa zgodna z folderem.
Odkrywalność25 / 25
Opis mówi, kiedy użyć skilla, ma sensowną długość i jest w 3. osobie.
Treść35 / 35
Co najmniej 150 słów i do 500 linii, nagłówki, listy kroków, przykłady albo kod.
Higiena15 / 15
Bez zaślepek typu TODO, bez ścieżek Windows, z licencją.
Ryzykobrak sygnałów w skanie
- Pliki w paczce
- 1
- Skrypty
- 0
- Komentarze HTML
- 0
- Adresy URL w SKILL.md
- 0
Przestarzałość
Brak sygnałów. Repozytorium zmienione 23.10.2026, bez odwołań do wycofanych modeli i API.
Licencja
GPL-3.0, otwarta.
Co robi i kiedy
Wykonuje plan rozmieszczenia elementów na schemacie elektronicznym i wprowadza zmiany w istniejącym schemacie.
Oryginalny opis (EN)
Use when executing a schematic placement plan (plan mode) or modifying an existing schematic (modification mode).
Jak działa
- Response Format
- Two Modes
- Error Handling — Escalate, Don't Improvise
- Checklist (Plan Mode)
- Rationalization Prevention
- Exit Gate
- Placement Spacing Reference
- Wiring Strategy Reference
- Power and Ground
- Naming
Sekcje z nagłówków SKILL.md, w oryginale · 362 linii, 2 883 słów
Podgląd SKILL.md
---
name: schematic-design
description: >
Use when executing a schematic placement plan (plan mode) or
modifying an existing schematic (modification mode).
---
<CRITICAL-RULE>
NEVER use the Read, Write, or Edit tools on KiCad files (.kicad_sch,
.kicad_pcb, .kicad_sym, .kicad_mod, .kicad_pro, .kicad_prl). ALL
KiCad file manipulation MUST go through the kicad MCP tools. NEVER
run kicad-cli commands via Bash. If an MCP tool returns an error, try
different parameters — do NOT fall back to manual file editing.
EVERY KiCad operation has a corresponding MCP tool. Do NOT claim a
tool does not exist without first listing all available tools. Key
tools that MUST be used instead of file writes:
- `add_symbol` — create custom symbol definitions in .kicad_sym files
- `create_symbol_library` — create new .kicad_sym library files
- `create_schematic` — create new .kicad_sch files
- `create_project` — create new .kicad_pro project files
If you find yourself thinking "there's no MCP tool for this," you are
wrong. Check the tool list again.
</CRITICAL-RULE>
# KiCad Schematic Design — Plan Executor
This skill executes schematic plans mechanically. All intelligence
(component selection, coordinate calculation, wiring decisions)
happened in prior phases. This skill reads a plan and executes it.
## Response Format
When this skill activates, announce the mode:
- **Plan mode:** Print exactly: "Using schematic-design to execute
the placement plan."
- **Modification mode:** Print exactly: "Using schematic-design to
modify the existing schematic."
Then proceed directly to the pre-flight checks for the appropriate
mode. Do not ask the user what to do — the plan or user instructions
are the input. Report progress as each placement/wiring step
completes, but keep updates brief (one line per step).
## Two Modes
### Plan Mode (new designs)
Reads `specs/schematic-plan.md` and executes mechanically. The plan
file is the sole source of truth — ignore prior conversation context
about how the plan was created. Read the plan, execute the plan.
**Pre-flight checks:**
1. Verify `specs/schematic-plan.md` exists and its reviewer returned
APPROVED
2. Read page size from plan, call `set_page_size` immediately if
not A4
3. Verify project/schematic files exist (create if needed)
4. If plan references custom symbol library, verify it exists via
`list_lib_symbols`
**Execution order:**
1. Project setup (`create_project`, `create_schematic`, etc.)
2. Set page size (if plan specifies non-A4)
3. Register symbol libraries (`create_sym_lib_table`)
4. Create custom symbols (`add_symbol`)
5. Place all components (`place_component` per coordinate table)
6. Wire all connections per wiring table — group all pins for the
same net into a single `wire_pins_to_net` call
7. Add no-connect flags
8. Add power flags
9. Add hierarchical sheets (if applicable)
10. Annotate — run `annotate_schematic` to assign reference designators.
For hierarchical designs, pass `project_path` to avoid cross-sheet
ref conflicts.
11. Validate hierarchy — run `validate_hierarchy` from root to check
for orphaned labels, direction mismatches, duplicate refs,
junctions and bus entry ends left inside wires, and flags and wire
ends left off the pins of mirrored, rotated parts; for each issue
with a `repair`, make that call (one with a `note` instead: see
the verification skill).
12. Run ERC
### Modification Mode (existing schematics)
No plan artifact required. User instructions serve as the plan.
**Pre-flight checks:**
1. Verify the schematic file exists
2. List current components via `list_schematic_components`
3. For each new component to be added, call `list_lib_symbols` to
verify its lib_id exists before placement
Follow existing spacing/wiring/naming conventions in the schematic.
## Error Handling — Escalate, Don't Improvise
| Situation | Response |
|-----------|----------|
| Symbol not found | STOP. Do not fuzzy-match or substitute. Report the error. If a previously-verified symbol is missing, instruct the user to re-run from circuit-design to re-validate the BOM. |
| Position outside page bounds | STOP. Report error. The plan's page calculation should have prevented this. Instruct the user to re-run schematic-plan. |
| connect_pins fails | Try wire_pins_to_net for that connection. If that fails, report and continue with remaining wiring. |
| `wire_pins_to_net` refuses | Act on the bracketed code, per the table below. |
| ERC violations | Report violations. Invoke verification skill. |
### `wire_pins_to_net` refusals
A refused call writes nothing and lists every refused pin with a
bracketed code, the obstacle and a remedy. Fix the cause and call
again with the same pins. Never work around a refusal with `add_label`
or `add_wires`: they check none of this, so they can merge nets
silently.
| Code | Meaning | Do this |
|------|---------|---------|
| `validation` | An argument is malformed: an empty or padded name, a leading `/`, `${`, a KiCad auto-name such as `Net-(...)`, bus syntax, an unknown direction, a stub not a multiple of 1.27 mm or over 1000 mm | Fix the argument |
| `resolve` | The reference is not on this sheet, the pin does not exist, or a pin name matches pads at different points | Pass the pad numbers the message lists, or wire the pin on the sheet that holds its unit |
| `names` | The pin's net already carries another name | If that name is a `Net-(...)` label `connect_pins` wrote, remove it with `remove_label` as the message says, then call again. If the pin belongs on the net, call again with its name as the message shows it; otherwise stop and report |
| `touch` | Every stub and label position would touch something | Pass another `direction`, or move the part; otherwise stop and report |
| `netclass` | Wiring would move a net into another net class | Stop and report |
| `nc_type` | The pin is a no-connect type pin | Pick another pin |
| `nc_flag` | The pin has a no-connect flag | If it should be connected, `remove_no_connect`, then call again |
| `dup_ref` | Another part shares the reference somewhere in the hierarchy, or a sheet of the hierarchy cannot be read, so sharing cannot be ruled out | Give each part its own reference (`annotate_schematic` numbers `?` references), then call again. For an unreadable sheet, stop and report which one the message names |
| `bus`, `bus_entry`, `sheet_pin`, `text_var`, `jumper`, `unit0_unplaced`, `units_disagree` | The pin's net may reach something this tool cannot judge | Stop and report |
| `derived`, `unloadable` | A symbol on the sheet has pins KiCad's file does not define, or defines twice, or an angle KiCad cannot load | Stop and report |
When `auto_place_decoupling_cap` meets one of these after placing the
cap, its error says what it left on disk and the calls that remove it;
any library symbol it copied into the file stays, and no net depends on
it.
## Checklist (Plan Mode)
**IMPORTANT: Use TodoWrite to create todos for EACH checklist item below.**
- [ ] Verify `specs/schematic-plan.md` exists and is APPROVED
- [ ] Pre-flight: verify project/schematic files exist
- [ ] Set page size (if non-A4)
- [ ] Register symbol libraries
- [ ] Create custom symbols (if needed)
- [ ] Place all components per coordinate table
- [ ] Wire all connections per wiring table
- [ ] Add no-connect flags
- [ ] Add power flags and PWR_FLAG symbols
- [ ] Annotate schematic — no `?` refs remaining
- [ ] Validate hierarchy — no orphaned labels or duplicate refs
- [ ] Run ERC — must show zero violations
## Rationalization Prevention
| Thought | Reality |
|---------|---------|
| "This pin name is close enough" | Use the exact pin name from the plan. The plan was verified against `get_symbol_info`. |
| "I can adjust the coordinates slightly" | Use the exact coordinates from the plan. The plan was verified against page bounds. |
| "I'll add an extra component not in the plan" | Do not improvise. If the design needs changes, go back to schematic-plan. |
| "The plan is probably outdated, I'll adapt" | The plan is the source of truth. If it's wrong, re-plan. Don't patch on the fly. |
## Exit Gate
Run `run_erc`. Zero violations → proceed to pcb-layout.
Violations → invoke verification skill.
**Commit strategy:** Commit after schematic-design completes and
ERC passes (not after each chunk). If ERC fails, fix violations via
verification skill, then commit the clean state. Do not commit
intermediate broken states.
## Placement Spacing Reference
All coordinates are on the 1.27mm grid (auto-snapped by the tools).
Minimum spacing (for modification mode and plan verification):
- **Vertical between components**: 10.16mm (8 grid units)
- **Horizontal between passives in a row**: 12.7mm (10 grid units)
- **IC to its supporting passives**: 25.4mm (20 grid units) horizontal
- **Between functional stages**: 25.4–50.8mm gap
Title block clearance: ~108x32mm at bottom-right corner. On A4
landscape (297x210mm), keep components within X < 180mm and
Y < 175mm.
## Wiring Strategy Reference
**Use `connect_pins`** (direct Manhattan wire) when:
- Two pins are within ~25mm of each other
- The wire path is visually obvious (one L-shaped segment)
**Use `wire_pins_to_net`** (batch: multiple pins to one net label) when:
- A net connects 3 or more components that are not all adjacent
- The net spans across functional stages
- Power and ground rails — always use net labels, never daisy-chain
What `wire_pins_to_net` writes: a short stub away from each pin with
the label at its end, or the label on the pin end when the stub would
touch something. It never writes a junction, and a pin already on the
net is left alone. Read the result's notes: "new local net" means
nothing on this sheet carried that name, so a power symbol or global
label of that name elsewhere does not join it (use `add_power_symbol`
or `add_global_label` to reach those); on a sheet used more than once,
the wiring lands in every instance, and the note names each one.
## Power and Ground
- Use `add_power_symbol` for VCC, GND, and named power rails
- Use `wire_pins_to_net` for custom power nets (VIN_PROT, 5V_REL, etc.)
- Place decoupling capacitors visually adjacent to the IC they serve
- Add `PWR_FLAG` on every power net that would otherwise trigger
"power pin not driven" ERC errors
- No tool places a PWR_FLAG for you, because only you know which nets have a
source ERC cannot see. Place one with `add_power_symbol`
(lib_id `power:PWR_FLAG`), once per net that needs it
- PWR_FLAG is only needed on nets with power_in pins and NO power_out/output pins.
Do not add one to a net that already has a driver or a flag: ERC then reports
two power outputs connected
## Naming
- Use **uppercase descriptive names** for nets: VIN_PROT, 5V_REL,
SPI_MOSI
- Active-low signals: suffix with `_N` (e.g., RESET_N, CS_N)
- Do not use generic names like NET1 or WIRE3
## MCP Tools for This Skill
**Reading / inspection:**
- `get_schematic_summary` — get item counts for a sheet
- `list_schematic_components` — list symbols on a sheet
- `list_schematic_labels` — list net labels on a sheet
- `list_schematic_wires` — list wires on a sheet
- `list_schematic_global_labels` — list global labels on a sheet
- `list_schematic_hierarchical_labels` — list hierarchical labels on a sheet
- `list_schematic_sheets` — list hierarchical sheet blocks on a sheet
- `list_schematic_junctions` — list junctions on a sheet
- `list_schematic_no_connects` — list no-connect flags on a sheet
- `list_schematic_bus_entries` — list bus entries on a sheet
- `get_symbol_pins` — get pin names and types for a placed symbol
- `get_pin_positions` — get placed pin coordinates (for wiring)
- `get_net_connections` — trace a net to see what's connected
- `list_unconnected_pins` — find pins that need wiring or no-connect
**Placing components:**
- `place_component` — place a symbol instance on the schematic
- `move_component`: move or turn a placed component. Its fields travel with it, wires stay put and the result names the pins whose connections changed; called at the symbol's own position it turns the symbol in place. Place and move parts before wiring, and after a move reconnect the pins the result names.
- `remove_component` — delete a placed component
- `set_component_property` — change reference, value, footprint, etc.
- `set_page_size` — resize the schematic sheet
- `add_lib_symbol` — load a symbol from a library into the schematic
**Wiring and connectivity:**
- `connect_pins` — direct Manhattan wire between two pins
- `wire_pins_to_net` — connect multiple pins to a named net label
- `add_wires` — add raw wire segments by coordinate
- `add_label` — place a net label
- `add_global_label` — place a global (cross-sheet) label
- `add_junctions` — add junction dots at wire intersections
- `no_connect_pin` — mark a pin as intentionally unconnected (idempotent)
- `remove_no_connect` — clear no-connect flag(s) from a pin
- `remove_label` / `remove_wire` / `remove_junction` — cleanup (labels and global labels)
**Power and decoupling:**
- `add_power_symbol` — place VCC, GND, +3V3, PWR_FLAG, etc.
- `auto_place_decoupling_cap` — auto-place a decoupling cap near an IC
**Annotations and hierarchy:**
- `add_text` — add text annotations to the sheet
- `add_hierarchical_label` — add a hierarchical label for sheet-to-sheet connections
- `remove_hierarchical_label` — remove a hierarchical label by name or UUID
- `modify_hierarchical_label` — modify text, shape, or position of a hierarchical label
- `annotate_schematic` — auto-assign reference designators (project server)
- `remove_text` — remove text annotations by position or content
**Hierarchy management (project server):**
- `add_hierarchical_sheet` / `remove_hierarchical_sheet` — create/remove sub-sheet blocks
- `modify_hierarchical_sheet` — change sheet name, file, dimensions (pins, fields and the wires
on pins follow a resize; a size below what the pins need is refused)
- `add_sheet_pin` / `remove_sheet_pin` — manage pins on sheet blocks
- `validate_hierarchy` — check for orphaned labels/pins, direction mismatches
and junctions and bus entry ends left inside wires, and flags and
wire ends left off the pins of mirrored, rotated parts, with the call
that repairs each where a tool can
- `list_hierarchy` / `get_sheet_info` — inspect hierarchy structure
- `is_root_schematic` — check if a schematic is root or sub-sheet
- `move_hierarchical_sheet` — reposition a sheet block on the canvas
- `reorder_sheet_pages`: change the page numbers, and so the page order, of hierarchical sheets
(call it on the root schematic)
- `duplicate_sheet`: create a copy of a sheet with new UUIDs and its own part references
(a sheet that has sub-sheets of its own is refused)
- `flatten_hierarchy`: write a single flat schematic whose netlist is the hierarchy's; it
refuses, writing nothing, where it could not keep that (bus names on sheet pins or in
sub-sheets, for one)
- `trace_hierarchical_net` — trace a net across the hierarchy for debugging
- `export_hierarchical_netlist` — export netlist with hierarchy info
(use instead of `export_netlist` for hierarchical designs)
## Hierarchy Workflow Sequences
### Sequence: Setting up a hierarchical design
1. `add_hierarchical_sheet` — create the sub-sheet block on the parent
2. `add_sheet_pin` — add pins to the sheet block for each signal crossing the boundary
(an edge with no free slot is refused with the height that fits; grow the sheet with
`modify_hierarchical_sheet` first)
3. In the child schematic: `add_hierarchical_label` for each pin
4. `validate_hierarchy` — verify pins match labels, no orphans
### Sequence: Duplicating a channel (e.g., 4 identical sensor channels)
1. Design the first channel as a sub-sheet
2. `duplicate_sheet`: creates a copy with new UUIDs, a new file and its own part references
(the first free number of each prefix), so the copy needs no annotation
3. Repeat for each additional channel
4. `validate_hierarchy` from the root: confirms no reference is shared across the copies
### Sequence: Pre-ERC annotation and validation
1. `annotate_schematic` with `project_path` — assign refs to all `?` components
2. `validate_hierarchy` from root — check for duplicates, orphans, mismatches
3. If duplicates: `set_component_property` to reset to `X?`, then re-annotate
4. `run_erc` — only after validate_hierarchy is clean
### Sequence: Debugging cross-sheet connectivity
1. `trace_hierarchical_net` — follow the net across sheet boundaries
2. `get_net_connections` — check connections on each sheet
3. `list_cross_sheet_nets` — see all nets crossing boundaries
4. Fix with `add_sheet_pin`, `add_hierarchical_label`, or `connect_pins`
### Sequence: Restructuring hierarchy
1. `flatten_hierarchy`: merge all sheets into one new file whose netlist is the hierarchy's; the
hierarchy is left alone, and a design it cannot flatten faithfully is refused
2. OR `move_hierarchical_sheet` — reposition sheet blocks on the parent
3. OR `reorder_sheet_pages` on the root: change the page numbers the sheets are ordered by
4. `validate_hierarchy` — verify structure is still valid
### Sequence: Cleaning up after modifications
1. `remove_text` — delete temporary text annotations
2. `validate_hierarchy` — check for new orphaned labels or direction mismatches
3. `annotate_schematic` — reassign any `?` refs introduced during modifications
**Verification and export:**
- `run_erc` — run electrical rules check
- `export_schematic` — export schematic as PDF/SVG
- `export_netlist` — generate a netlist file (PCB import itself is `update_pcb_from_schematic` on the PCB server)
- `export_bom` — export bill of materials
**Symbol authoring (when a part isn't in KiCad's libraries):**
- `create_symbol_library` — create a project-local .kicad_sym file
- `add_symbol` — define a custom symbol with pins, footprint, datasheet
- `list_lib_symbols` / `get_symbol_info` — browse available symbols
## Custom Symbols
When a part is not in KiCad's built-in libraries, create a custom
symbol using MCP tools — NEVER by writing .kicad_sym files directly:
1. `create_symbol_library` — create a project-local .kicad_sym file
(if it doesn't exist yet)
2. `add_symbol` — define the symbol with pin names, pin types, pin
numbers, footprint, and datasheet
3. `add_lib_symbol` — load the custom symbol into the schematic
## Verification
After completing placement and wiring:
1. Run `run_erc` to check for violations
2. Fix "power pin not driven" with PWR_FLAG symbols
3. Fix unconnected pins with `wire_pins_to_net` or `no_connect_pin`
3.5. If components have `?` references, run `annotate_schematic` with
`project_path` before re-running ERC.
4. Re-run ERC until clean
Wersje
W bazie nie ma innych skilli o nazwie schematic-design.
Migawka bazy z 13.11.2026 · wersja paczki 902a4ab66a50 (skrót SHA-256 całej paczki)
Pobrania w ostatnich 30 dniach: 0 · ranking
Zgłoś problem z tym skillem: szkodliwa treść, błędny opis albo prośba autora o usunięcie.
Podobne skille
- 100kicad-schematic
Prowadzi projektowanie schematów KiCAD przez narzędzia MCP: dodawanie komponentów i symboli, łączenie pinów, etykiety sieci i szyny zasilania. - 100schematic-webhooks
Odbiera i weryfikuje webhooki Schematic, w tym podpis X-Schematic-Webhook-Signature oraz zdarzenia firm lub subskrypcji. Przydaje się przy konfiguracji obsługi webhooków. - 90schematic-deep-review
Wyjaśnia pełne schematy elektroniczne przez sprawdzone połączenia, ścieżki zasilania i obliczenia, zbiera karty katalogowe i tworzy PDF z adnotacjami. - 100getting-started
Wprowadza w zestaw Schematic: instalację w Claude Code lub innej aplikacji, dobór skilla do zadania i otwieranie plików. - 100circuit-design
Projektuje obwody analogowe: dobór topologii, wymiarowanie metodą gm/Id, polaryzację, schemat, ERC i przegląd, od specyfikacji do schematu gotowego do akceptacji. - 82akcli-schematic-authoring
Tworzy nowy schemat KiCad z wymagań albo rozbudowuje arkusz, pisząc listę operacji akcli i pętlę: plan, próba, zastosowanie, weryfikacja.