Kicad Schematic

KiCAD Schematic Design Workflow

This skill guides Claude to design schematics using Konnect MCP tools. ALL modifications go through MCP tools — never edit .kicad_sch files directly.

Toolset Loading

Before any schematic work, load the required toolsets:

load_toolset('sch_components')   # place, move, rotate, delete symbols
load_toolset('sch_wiring')       # wires, net labels, power symbols, connections
load_toolset('sch_analysis')     # connection validation, short and orphan checks
load_toolset('sch_export')       # direct ERC and rendered schematic evidence
load_toolset('project')          # save_project before formal checks

Load additional toolsets as needed:

load_toolset('library')          # search_symbols, get_symbol_info, list_symbol_libraries
load_toolset('sch_batch')        # batch operations for 3+ items

Always call get_active_toolsets() first to see what is already loaded.

Component Placement

Read references/common-lib-ids.md when choosing a common generic KiCad symbol. It is a quick-start index, not an allowlist; search the active libraries when the required part is absent or package-specific.

Workflow

1. Search the library first: use search_symbols to find the correct lib_id
2. Get pin info: use get_symbol_info to see pin names, numbers, and positions
3. Place on the 1.27mm grid (KiCAD default schematic grid)
4. Verify placement with list_schematic_components

Package-sensitive and custom parts

Before placing or wiring a custom symbol, a manufacturer-specific discrete, or any package whose view can be mirrored, require the kicad-library skill's accepted physical pin map for the exact MPN and package suffix. The map must join each datasheet lead to the symbol pin and footprint pad, identify the drawing view/direction, reconcile duplicate and mechanical pads, and include query-back plus disposable rendered inspection. get_symbol_info proves the library data that exists; it does not prove that data matches the package.

If the accepted physical pin map is missing, incomplete, based on a different suffix, or ambiguous about top/bottom/mating view, stop before real schematic placement. Do not infer physical numbering from a generic symbol name or from the order pins appear on screen.

Common Library IDs

Rotation Conventions

• 0 degrees: default orientation (pins left/right)
• 90 degrees: rotated CCW (useful for vertical components)
• 180 degrees: flipped horizontally
• 270 degrees: rotated CW

Power symbols: GND uses 0 (arrow points down), VCC/VDD/+3V3/+5V use 0 (arrow points up).

Spacing Guidelines

• Between ICs: 30-50mm horizontal, 20-30mm vertical
• Between passive components: 10-15mm
• Between a decoupling cap and its IC: 5-10mm
• Leave room for wiring: minimum 5mm between component pins and other elements

Wiring

Read references/wiring-patterns.md when choosing between direct wires and labels or when building one of its common subcircuits. Verify every named pin against the placed symbol before applying a pattern.

Connection Methods — Decision Table

connect_pins

Use for direct pin-to-pin connections. The tool auto-routes with L-bends.

connect_pins(schematic, ref1, pin1, ref2, pin2)

• Specify pins by pin number (from get_schematic_pin_locations)
• Works best when pins are nearby and facing each other
• Automatically creates wire segments with proper bends

connect_to_net

Use for named nets. Creates a short stub wire and attaches a net label.

connect_to_net(schematic, reference, pin_number, net)

• Preferred for signals that connect to 3+ pins
• Preferred for named buses and control signals
• Keeps schematic clean and readable
• Net name must be consistent across all connections
• Name the pin rather than passing pin_x/pin_y: the stub then points away from the symbol body on its own, instead of the label text running back across the pin names. Override with direction only to fix a layout clash.
• batch_connect_to_net does the same for many pins in one read/write. By default it places its labels directly on the pin endpoints without stubs; pass stub_length, direction and label_type for connect_to_net's layout on every pin in the call.
• Placing a label by hand with add_schematic_net_label instead? Take its rotation from orientation_degrees in get_schematic_pin_locations, or the text reads back across the symbol's pin names.
• These labels are sheet-local. In a sheet placed more than once, each instance gets its own independent copy of the net — right for per-instance signals, wrong for a rail every instance must share. A shared rail takes add_power_symbol or add_schematic_net_label with label_type: global_label; both are one net across all sheets and instances.

add_power_symbol

Use for all power connections, in preference to labelling a pin with the rail name. The one exception is a rail that must stay separate per instance of a repeated sheet — see below.

add_power_symbol(schematic, power_net, x, y, rotation?)

• Takes coordinates, not a reference and pin number. Place it on the pin endpoint (from get_schematic_pin_locations) — a power symbol carries its pin at its own origin, so the two coinciding is the connection.
• The position is snapped to the 1.27mm grid, like every other placer, and the response reports where the symbol landed. Pin endpoints of placed components are already on that grid, so a pin endpoint is kept as given.
• power_net is loaded as power:<power_net>, so it must name a symbol in KiCad's power library: +3V3 and +12V, never 3V3 or 12V. A miss is an error and nothing is placed.
• rotation defaults to 0 — see Rotation Conventions above.
• A power pin landing mid-segment on a wire gets its junction dot automatically, in either order: symbol onto an existing wire, or a wire routed across an already-placed symbol.
• Power symbols are global: every +5V symbol on every sheet, and in every instance of a sheet, joins one +5V net. A rail that must stay separate per instance of a repeated sheet (each node's own 5V, say) takes a local net label via connect_to_net instead — power:+5V there shorts all the instances' rails together.

Batch Operations

Load sch_batch toolset when placing 3 or more components or making bulk connections.

batch_place_components

Place multiple components in one call. Provide schematic and a components array of {lib_id, x, y, rotation?, reference?, value?, unit?} objects. Pass reference explicitly for each component -- it is not auto-assigned.

The batch commits all symbols once, then reconciles every new pin endpoint in that same atomic write. Check the "junctions_added_count" and "junctions_pruned_count" response fields; a pin placed mid-segment on an existing wire is not electrically connected in KiCad unless the required junction was added.

batch_connect_to_net

Connect multiple pins to the same net in one call. Ideal for:

• Connecting all VCC pins on an IC
• Connecting all GND pins
• Bus signals across multiple ICs

batch_edit_schematic_components

Bulk-modify component properties (values, footprints, fields) across multiple components. The default remains update-only. Set create_missing: true to create a missing custom field on every placed unit of each named component. Reference, Value, Footprint and Datasheet are never created through this option; use the dedicated arguments or workflows for built-in fields. Inspect each result's “updated_units” and “created_units” counts, because a partially populated multi-unit component can report both.

When to Use Batch vs Individual

• 1-2 components: individual calls
• 3+ components: batch operations
• Mixed operations (place + wire): do placement batch first, then wiring batch

Common Patterns

Decoupling Capacitor

Place 100nF cap (Device:C) within 5mm of IC power pin. Connect one pin to VCC via power symbol, other pin to GND via power symbol. One cap per VCC/VDD pin.

Pull-up Resistor

Place resistor (Device:R) vertically. Connect one pin to the signal net via connect_to_net, other pin to VCC via add_power_symbol. Typical values: 4.7k for I2C, 10k for general.