KiCAD PCB Layout Workflow

This skill guides Claude to perform PCB layout using Konnect MCP tools. ALL modifications go through MCP tools — never edit .kicad_pcb files directly.

---

Prerequisites

Most PCB layout operations require KiCAD to be running with the board file open. The IPC connection communicates with the running KiCAD instance in real-time.

Some board-construction and component tools have guarded closed-board paths. IPC-first tools fall back to the file only when the transport is unreachable and the target board has not been observed live during this server session. File-only operations such as flip_component proceed only when KiCad does not hold the target board open. These paths use revision-aware atomic writes: placement preserves pads, graphics, attributes, and models; moves preserve the existing angle; rotations update the footprint and its child angles; flips mirror supported geometry and swap front/back layers. A reachable KiCad rejection stays closed instead of racing the editor.

unsafe_file_fallback is a stop condition. It means Konnect reached this board live earlier in the current server session but IPC is now unreachable, so the saved file may be older than lost editor state. Pause mutation work, tell the user that Konnect left the file unchanged, and ask them to reopen/recover, reconcile, and save the board in KiCad. Continue through live IPC afterward. Preserve the guard: do not retry-loop, restart Konnect automatically, or edit .kicad_pcb directly. If the user confirms a clean close and an authoritative saved file, they may restart Konnect to deliberately begin a new closed-board session.

If connection fails:

• Tell the user to open KiCAD and load the project
• The board (.kicad_pcb) must be open in the PCB editor
• KiCAD's IPC API must be enabled (default in KiCAD 8+)

---

Toolset Loading

Before any PCB work, load the required toolsets:

load_toolset('pcb_board')        # board outline, layers, setup, stackup
load_toolset('pcb_components')   # place, refresh, move, rotate, align footprints
load_toolset('pcb_routing')      # traces, vias, differential pairs
load_toolset('sch_export')       # update PCB from the saved schematic hierarchy

Zones (pcb_board: add_zone; pcb_routing: add_copper_pour), component/net queries (pcb_components: find_component, get_component_list; pcb_board: get_board_info), and bulk placement (pcb_components: place_component_array, align_components, duplicate_component) are already covered by the toolsets loaded above.

Load additional toolsets as needed:

load_toolset('config')           # design rule storage: add_design_rule, list_design_rules
load_toolset('verification')     # run_drc, set_design_rules, set_predefined_sizes, check_clearance

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

References by decision

• Read references/layer-reference.md when selecting a copper, fabrication, user, or mechanical layer or deciding which side owns an item.
• Read references/trace-width-table.md when sizing a current-carrying trace, via, or controlled-impedance route. It defines the required calculation inputs and acceptance record; it is not a lookup table.
• Read references/design-rules.md when creating netclasses, configuring project constraints, or adjudicating DRC results.

---

Layout Order

Follow this sequence for a clean PCB workflow:

1. Board outline — set_board_size or draw Edge.Cuts geometry. Both outline tools append, so resize with delete_graphics(layer='Edge.Cuts') first — a second call without it leaves two overlapping outlines and a DRC failure.
2. Update from schematic — call update_pcb_from_schematic first with dry_run: true. Review status, coverage, diagnostics, and staged positions. Apply only with dry_run: false and the exact returned expected_plan_revision value. The saved schematic hierarchy must be closed in the schematic editor, and the target board must be open in KiCad. A conflict is non-mutating; resolve it and rerun the dry run. A successful apply is one KiCad undo entry, so Ctrl-Z reverses the whole update.
3. Refresh changed libraries — when a linked footprint library changed, use update_footprints_from_library, the MCP equivalent of KiCad Tools → Update Footprints from Library. This is distinct from update_pcb_from_schematic: it refreshes supported library-owned pads, graphics, attributes, metadata, and 3D models without changing references, placement, side, rotation, KIID, symbol metadata, instance overrides, or pad nets. Always call it first with dry_run: true; apply only with dry_run: false and the exact returned expected_plan_revision. The requested board must be open in live KiCad, one apply is one undo entry, and unsupported or stale content returns a non-mutating conflict instead of silently dropping it.
4. Place components — position all footprints
5. Route traces — connect all nets
6. Copper pour — add ground/power zones last
7. DRC — run design rule check
8. Save — save_project

Do NOT add copper pours before routing is complete — they interfere with interactive routing.

---

Placement

Strategy

• Group components by functional block (power, digital, analog, connectors)
• Place ICs first, then their associated passives
• Decoupling caps: within 2mm of their IC power pins, on same layer
• Cable/EMI filter caps: on the connector's own pins, and judged against that connector rather than the nearest IC
• Connectors: at board edges, accessible for cables
• High-frequency components: minimize trace lengths between them
• Thermal considerations: power components away from sensitive analog

Placement Tools

Tool	Use Case
place_component	Position one footprint via IPC or safe file fallback
update_footprints_from_library	Refresh placed definitions from linked libraries
move_component	Relocate a footprint via IPC or safe file fallback
rotate_component	Rotate a footprint via IPC or safe file fallback
flip_component	Set F.Cu/B.Cu on a closed board with geometry mirroring
align_components	Align multiple components (top/bottom/left/right/center)
place_component_array	Grid placement for repeated elements

Score-first automation

Load load_toolset('placement') for the automation loop. The discipline is score, change, re-score — every planner reports the board's score before and after its own plan, so a change is judged before it is made:

1. score_placement — 0-100 with named deductions; hard failures (courtyard overlaps, parts outside the outline) decide the verdict regardless of the number, and a board with no outline can never pass. interface_filter_caps lists caps that were within their family limit of a connector carrying every one of their nets: that is cable filtering, so the decoupling rule was answered rather than skipped. They are not defects to "fix" by dragging them toward an IC.
2. auto_place_from_schematic — deterministic first placement by net clusters; explicitly a starting point, not a final layout.
3. refine_placement_force_directed — deterministic spring embedder; pass locked for parts that must not move. Same input, same plan.
4. place_decoupling_caps — plans a row beside an IC, paired by shared nets.
5. plan_bga_fanout — pitch detected from the pad grid; apply executes as one KiCad undo commit over live IPC.

Every planner is dry-run by default; apply refuses while KiCad holds the board open live (fanout apply is the inverse: it REQUIRES the live board).

Placement Tips

• Use mm coordinates (KiCAD default for PCB)
• Standard grid: 0.5mm for placement, 0.25mm for fine adjustment
• Check component courtyard overlaps after placement
• Reference designator text: F.SilkS layer, 1mm height default

---

Routing

Routing Tools

Tool	Use Case
route_pad_to_pad	Direct connection, auto L-bend routing
route_trace	Manual segment-by-segment routing
route_differential_pair	Matched-length USB/LVDS/Ethernet pairs
add_via	Layer transition
create_netclass	Define width/clearance rules for net groups

route_pad_to_pad

The primary routing tool. Looks up both pad positions on the board and lays an L-shaped trace between them.

route_pad_to_pad(board, net_name, ref1, pad1, ref2, pad2, layer?, width?)

• Emits one segment when the pads already share an X or Y, two otherwise
• Specify the width in mm from the accepted project netclass or sizing record.
• Routes entirely on layer (default F.Cu) — it does not add a via. To change layer mid-route, place the via yourself with add_via and route each side separately

route_trace

One straight segment between two explicit points, for when you want to control the path yourself.

route_trace(board, net_name, layer, x1, y1, x2, y2, width?)

• Use when auto-routing creates suboptimal paths
• There is no waypoint list: call it once per segment to build a polyline
• Coordinates are board-space mm

route_differential_pair

For differential signals (USB, HDMI, Ethernet, LVDS).

route_differential_pair(board, net_pos, net_neg, x1, y1, x2, y2, gap?, layer?, width?)

• Lays two straight traces parallel to the given line, offset (gap + width)/2 either side, so spacing is constant along the segment
• Not a length-matching router: it adds no serpentine tuning, and equal length only follows from the two traces being parallel segments. Skew introduced before or after this call is yours to correct
• Common pairs: USB_D+/USB_D-, LVDS_P/LVDS_N

Netclasses

Define routing rules for groups of nets:

create_netclass(board, name, trace_width?, clearance?, via_drill?, via_diameter?)

The class is written to the project's .kicad_pro file, which is where KiCad has kept netclasses since v7 — the board file is not modified.

Before creating or updating a class, read get_netclasses and the applicable design-rule/trace-sizing references. Derive width, clearance, gap, drill, and diameter from the selected fabrication contract, stackup, and electrical calculation. Read the classes back after the write and confirm every special net resolves through the intended class. Missing inputs make the rule INCOMPLETE.

Pre-defined sizes

Netclass width is the default. The Track/Via dropdowns are a separate palette in the sibling .kicad_pro. Fill them with set_predefined_sizes so W / Shift+W can step through extra widths without changing netclasses:

The values below show call syntax only; they are not engineering recommendations. Replace every value with one from the accepted project sizing record, derived from the current fabrication contract, stackup, and electrical requirements. If that evidence is unavailable, report the sizing task as INCOMPLETE instead of reusing these illustrative values.

set_predefined_sizes(board, track_widths=[0.2, 0.5, 0.8],
    via_dimensions=[{diameter:0.6, drill:0.3}, {diameter:0.8, drill:0.4}])

A leading 0 mm / 0,0 via is always kept as “use netclass values”. These sizes are not DRC limits. KiCad reads the list on next project open.

---

Copper Pour

Zone tools live in the pcb_board toolset.

add_zone

Creates a copper pour area (polygon fill).

add_zone(board, net_name, layer, points, clearance?, min_width?,
         name?, priority?, pad_connection?)

• Almost always GND net on both F.Cu and B.Cu
• points is the outline polygon; define it slightly inside the board edge (0.5mm inset)
• priority defaults to 0; the higher priority wins where two pours overlap
• pad_connection is solid | thermal | none, defaulting to thermal as KiCad does
• With KiCad running on this board the zone is created over IPC and refilled for you, so it appears at once and is in KiCad's undo stack. Without a live KiCad it goes into the file instead, and the result says so (source: file) and carries a warning describing the process-local evidence and cold-start limitation. A board observed live earlier in this server session fails with unsafe_file_fallback instead of writing the file.

refill_zones

Must call refill_zones after any change that affects copper pour:

• After adding/moving components
• After routing new traces
• After modifying zone outlines
• After changing design rules

Zones do not auto-update — stale fills cause DRC errors.

Zone Tips

• GND pour on both layers is standard practice
• Leave spoke thermal reliefs for through-hole pads (easier soldering)
• Use keepout zones to prevent copper in sensitive areas
• Zone clearance typically 0.3-0.5mm from traces

---

Layer Reference

Layer	Name	Purpose
F.Cu	Front Copper	Top copper traces and pads
B.Cu	Back Copper	Bottom copper traces and pads
F.SilkS	Front Silk	Top silkscreen (text, outlines)
B.SilkS	Back Silk	Bottom silkscreen
F.Mask	Front Mask	Top solder mask openings
B.Mask	Back Mask	Bottom solder mask openings
Edge.Cuts	Board Outline	Physical board boundary
F.Fab	Front Fab	Top fabrication drawing
B.Fab	Back Fab	Bottom fabrication drawing
F.CrtYd	Front Courtyard	Top component clearance area
B.CrtYd	Back Courtyard	Bottom component clearance area
In1.Cu	Inner 1	Internal copper layer 1
In2.Cu	Inner 2	Internal copper layer 2

Layer Usage Guidelines

• Route signals on F.Cu and B.Cu (2-layer) or add inner layers for complex boards
• Board outline MUST be on Edge.Cuts (closed polygon or rectangle)
• Silkscreen for reference designators and polarity marks
• Courtyard defines minimum spacing between components
• Use F.Fab/B.Fab for assembly drawings and component outlines

---

Design Rule Check

After completing layout:

run_drc()

Common DRC errors and fixes:

• Clearance violation: move trace or component further apart
• Unconnected net: route missing connection
• Track too close to edge: move inward from board outline
• Courtyard overlap: increase spacing between components
• Zone fill error: run refill_zones

---

Rules

1. Never edit .kicad_pcb directly — all changes go through MCP tools
2. Always verify placement after moves — components may snap to unexpected positions
3. Board outline first — define the physical boundary before placing anything
4. Refill zones after changes — stale zone fills cause phantom DRC errors
5. Check DRC before finishing — run run_drc() and resolve all errors
6. Use netclasses for consistency — define track widths per net type, not per trace
7. KiCAD normally must be running — use guarded closed-board paths only when a tool explicitly offers them. Treat unsafe_file_fallback as a human recovery boundary; other PCB edits still require the live IPC connection.
8. Save frequently — call save_project after major operations
9. Load toolsets first — check get_active_toolsets() and load what you need
10. Copper pour last — add zones only after routing is substantially complete