nearxos/kicad-mcp-server
1
0
Fork 0
Code Issues Pull Requests Actions Packages Projects Releases Wiki Activity

fix(sync_schematic_to_board): add missing footprints, not just nets (#171)

Browse Source 
The handler iterated `board.GetFootprints()` and assigned nets to existing
pads, but had no path to *add* footprints for schematic symbols whose
Reference was not yet on the board. New parts placed on the schematic
landed in the net list with no PCB representation — the rats nest had
nowhere to terminate, and place_component / route_pad_to_pad would fail
because the target footprint did not exist.

KiCad's "Update PCB from Schematic" (F8) implicitly adds the missing
footprints; bring the MCP's behaviour in line.

Implementation:
* `_extract_components_from_schematic` runs `kicad-cli sch export netlist
  --format kicadxml` (the same path `_handle_generate_netlist` already
  uses) and returns a flat `[{reference, value, footprint}]` list. Walks
  hierarchical sub-sheets transparently because kicad-cli does.
* `_add_missing_footprints_from_schematic` resolves each missing component
  against the project's fp-lib-table via `LibraryManager`, calls
  `pcbnew.FootprintLoad`, sets reference / value / FPID, and places the
  footprint at the board origin (the user / autoplacer can position it).
  Power and flag references (`#PWR…`, `#FLG…`) are excluded — they have
  no PCB footprint.
* The pad-net assignment loop now runs *after* the add path, so newly
  placed footprints get their nets assigned in the same call.
* Response payload gains `footprints_added` and `footprints_skipped`
  diagnostic lists. The textual `message` field reports both the new
  footprint count and the existing net / pad counts.

Adds tests/test_sync_schematic_to_board_footprints.py — 9 unit tests
covering the add path (missing ref, already-present ref, power refs,
empty footprint, unknown library) and the kicad-cli helper (XML parse,
missing kicad-cli, non-zero exit).
This commit is contained in:
Matthew Runo
2026-05-18 11:05:22 -07:00
committed by GitHub
parent e66c13361b
commit 679ccbf744
2 changed files with 489 additions and 3 deletions
Download Patch File Download Diff File Expand all files Collapse all files

170
python/kicad_interface.py
View File

@@ -4181,6 +4181,15 @@ class KiCADInterface:
# Build hierarchical pad→net map (walks all sub-sheets)
pad_net_map, net_names = self._build_hierarchical_pad_net_map(schematic_path)
# Add missing footprints from the schematic to the board *before*
# we add nets and assign pads — F8 in KiCad does this implicitly
# ("Update PCB from Schematic"), but our previous implementation
# only mutated nets, leaving newly-added schematic symbols with no
# PCB footprint at all.
added_footprints, skipped_footprints = self._add_missing_footprints_from_schematic(
board, schematic_path
)
# Add all nets to board
netinfo = board.GetNetInfo()
nets_by_name = netinfo.NetsByName()
@@ -4195,7 +4204,7 @@ class KiCADInterface:
netinfo = board.GetNetInfo()
nets_by_name = netinfo.NetsByName()
# Assign nets to pads
# Assign nets to pads (now also covers any footprints we just added)
assigned_pads = 0
unmatched = []
for fp in board.GetFootprints():
@@ -4219,15 +4228,21 @@ class KiCADInterface:
self._update_command_handlers()
logger.info(
f"sync_schematic_to_board: {len(added_nets)} nets added, {assigned_pads} pads assigned"
f"sync_schematic_to_board: {len(added_nets)} nets added, "
f"{len(added_footprints)} footprints added, {assigned_pads} pads assigned"
)
return {
"success": True,
"message": f"PCB nets synced from schematic: {len(added_nets)} nets added, {assigned_pads} pads assigned",
"message": (
f"PCB updated from schematic: {len(added_footprints)} footprints added, "
f"{len(added_nets)} nets added, {assigned_pads} pads assigned"
),
"nets_added": added_nets,
"nets_total": len(net_names),
"pads_assigned": assigned_pads,
"unmatched_pads_sample": unmatched[:10],
"footprints_added": added_footprints,
"footprints_skipped": skipped_footprints,
}
except Exception as e:
@@ -4237,6 +4252,155 @@ class KiCADInterface:
logger.error(traceback.format_exc())
return {"success": False, "message": str(e)}
def _extract_components_from_schematic(self, schematic_path: str) -> List[Dict[str, str]]:
"""Run kicad-cli netlist export and return the flat list of components.
Each entry: {"reference": str, "value": str, "footprint": str}
Empty list on any failure (kicad-cli missing, parse error, etc.) — the
caller treats that as "no missing footprints to add".
"""
import subprocess
import tempfile
import xml.etree.ElementTree as ET
kicad_cli = self._find_kicad_cli_static()
if not kicad_cli:
logger.warning("kicad-cli not found — sync will not add new footprints")
return []
with tempfile.NamedTemporaryFile(suffix=".xml", delete=False) as tmp:
tmp_path = tmp.name
try:
cmd = [
kicad_cli,
"sch",
"export",
"netlist",
"--format",
"kicadxml",
"--output",
tmp_path,
schematic_path,
]
result = subprocess.run(cmd, capture_output=True, text=True, timeout=60)
if result.returncode != 0:
logger.warning(
f"kicad-cli netlist export failed (exit {result.returncode}): "
f"{result.stderr.strip()}"
)
return []
tree = ET.parse(tmp_path)
root = tree.getroot()
components = []
for comp in root.findall("./components/comp"):
components.append(
{
"reference": comp.get("ref", ""),
"value": comp.findtext("value", ""),
"footprint": comp.findtext("footprint", ""),
}
)
return components
except Exception as e:
logger.warning(f"Failed to extract components from schematic: {e}")
return []
finally:
try:
os.unlink(tmp_path)
except OSError:
pass
def _add_missing_footprints_from_schematic(
self, board: Any, schematic_path: str
) -> Tuple[List[Dict[str, str]], List[Dict[str, str]]]:
"""Add footprints to ``board`` for any schematic component not yet present.
New footprints are placed at the board origin so the user can move them
into position. Power/flag references (``#PWR``, ``#FLG``) are skipped —
they have no PCB representation.
Returns ``(added, skipped)``: each entry is
``{"reference": str, "footprint": str, "reason": str?}``.
"""
from pathlib import Path
from commands.library import LibraryManager
added: List[Dict[str, str]] = []
skipped: List[Dict[str, str]] = []
components = self._extract_components_from_schematic(schematic_path)
if not components:
return added, skipped
existing_refs = {fp.GetReference() for fp in board.GetFootprints()}
project_dir = Path(schematic_path).parent
library_manager = LibraryManager(project_path=project_dir)
for comp in components:
ref = comp["reference"]
fp_str = comp["footprint"]
if not ref or ref.startswith("#"):
# Power flags / global indicators — no PCB footprint expected.
continue
if ref in existing_refs:
continue
if not fp_str or ":" not in fp_str:
skipped.append(
{
"reference": ref,
"footprint": fp_str,
"reason": "no Library:Name footprint set on schematic symbol",
}
)
continue
lib_name, fp_name = fp_str.split(":", 1)
library_path = library_manager.libraries.get(lib_name)
if not library_path:
skipped.append(
{
"reference": ref,
"footprint": fp_str,
"reason": f"library '{lib_name}' not in fp-lib-table",
}
)
continue
try:
module = pcbnew.FootprintLoad(library_path, fp_name)
except Exception as e:
skipped.append(
{"reference": ref, "footprint": fp_str, "reason": f"FootprintLoad failed: {e}"}
)
continue
if not module:
skipped.append(
{
"reference": ref,
"footprint": fp_str,
"reason": f"footprint '{fp_name}' not in '{lib_name}'",
}
)
continue
module.SetReference(ref)
if comp["value"]:
module.SetValue(comp["value"])
module.SetFPID(pcbnew.LIB_ID(lib_name, fp_name))
# Place at board origin; user / autoplacer can position from there.
module.SetPosition(pcbnew.VECTOR2I(0, 0))
board.Add(module)
existing_refs.add(ref)
added.append({"reference": ref, "footprint": fp_str})
if added:
logger.info(f"_add_missing_footprints_from_schematic: added {len(added)} footprints")
return added, skipped
# ===================================================================
# Schematic analysis tools (read-only)
# ===================================================================