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

fix(add_mounting_hole): set FPID and restrict NPTH pad to mask layers (#154)

Browse Source 
`BoardOutlineCommands.add_mounting_hole` produced footprints with an empty
library:name id (`(footprint "" ...)` in the .kicad_pcb), which KiCad's GUI
Move tool refuses to select — users couldn't drag the resulting MHs in the
editor. It also emitted the pad with the default `*.Cu` + `*.Mask` LSET on
NPTHs; with `padDiameter > diameter` that creates phantom copper annular
rings on every Cu layer and trips clearance DRC against neighbouring nets.

Repro: call `add_mounting_hole` with `position={x:117,y:84.5,unit:"mm"},
diameter:3.2, padDiameter:3.5`. The resulting MH is unselectable and DRC
reports phantom F.Cu pad shorts to neighbouring component pads.

Changes:

- Set a real FPID via `module.SetFPID(pcbnew.LIB_ID(lib, name))`. Default
  is `MountingHole:MountingHole_<diameter:g>mm` (e.g. 3.2 → 3.2mm); a new
  optional `footprintLibId` parameter overrides.
- For NPTH (the default `plated:false`), restrict the pad's LSET to
  `F.Mask` + `B.Mask` only. PTH path is unchanged — the default Cu+Mask
  LSET is correct there.
- Update the schema in `tool_schemas.py`: previously advertised
  `x`/`y`/`diameter` at the top level, but the impl reads
  `position={x,y,unit}`, `padDiameter`, `plated`. Schema now matches the
  implementation and exposes the new `footprintLibId` param.
- New `tests/test_add_mounting_hole.py` regression suite (7 tests) asserting
  SetFPID is invoked with non-empty lib:name (default + override forms),
  NPTH SetLayerSet excludes any Cu layer, and PTH does not call
  SetLayerSet (preserves default Cu+Mask).
This commit is contained in:
Matthew Runo
2026-05-18 11:05:10 -07:00
committed by GitHub
parent ff6ae63b8c
commit 4740013d24
3 changed files with 249 additions and 5 deletions
Download Patch File Download Diff File Expand all files Collapse all files

27
python/commands/board/outline.py
View File

@@ -216,6 +216,7 @@ class BoardOutlineCommands:
diameter = params.get("diameter")
pad_diameter = params.get("padDiameter")
plated = params.get("plated", False)
footprint_lib_id = params.get("footprintLibId")
if not position or not diameter:
return {
@@ -247,6 +248,19 @@ class BoardOutlineCommands:
module.SetReference(f"MH{next_num}")
module.SetValue(f"MountingHole_{diameter}mm")
# Set a real library:name FPID. Without this, the footprint is
# written as `(footprint "" ...)` and KiCad's GUI Move tool refuses
# to select it (no library link → not draggable in the editor).
if not footprint_lib_id:
# Strip trailing zeros so 3.2 → "3.2" not "3.20"
footprint_lib_id = f"MountingHole:MountingHole_{diameter:g}mm"
if ":" in footprint_lib_id:
lib_name, fp_name = footprint_lib_id.split(":", 1)
else:
lib_name = "MountingHole"
fp_name = footprint_lib_id
module.SetFPID(pcbnew.LIB_ID(lib_name, fp_name))
# Create the pad for the hole
pad = pcbnew.PAD(module)
pad.SetNumber(1)
@@ -255,6 +269,18 @@ class BoardOutlineCommands:
pad.SetSize(pcbnew.VECTOR2I(pad_diameter_nm, pad_diameter_nm))
pad.SetDrillSize(pcbnew.VECTOR2I(diameter_nm, diameter_nm))
pad.SetPosition(pcbnew.VECTOR2I(0, 0)) # Position relative to module
if not plated:
# NPTH must not include *.Cu in pad layers. The default LSET
# for a circular pad is *.Cu + *.Mask; on a NPTH with
# padDiameter > diameter that produces phantom copper annular
# rings on every Cu layer, which trip clearance DRC against
# neighbouring nets.
mask_only = pcbnew.LSET()
mask_only.AddLayer(pcbnew.F_Mask)
mask_only.AddLayer(pcbnew.B_Mask)
pad.SetLayerSet(mask_only)
module.Add(pad)
# Position the mounting hole
@@ -271,6 +297,7 @@ class BoardOutlineCommands:
"diameter": diameter,
"padDiameter": pad_diameter or diameter + 1,
"plated": plated,
"footprintLibId": f"{lib_name}:{fp_name}",
},
}

37
python/schemas/tool_schemas.py
View File

@@ -266,19 +266,46 @@ BOARD_TOOLS = [
{
"name": "add_mounting_hole",
"title": "Add Mounting Hole",
"description": "Adds a mounting hole (non-plated through hole) at the specified position with given diameter.",
"description": "Adds a mounting hole at the specified position with given diameter. Defaults to non-plated (NPTH) with mask-only pad layers; set plated=true for a PTH with copper pad.",
"inputSchema": {
"type": "object",
"properties": {
"x": {"type": "number", "description": "X coordinate in millimeters"},
"y": {"type": "number", "description": "Y coordinate in millimeters"},
"position": {
"type": "object",
"description": "Position of the mounting hole",
"properties": {
"x": {"type": "number", "description": "X coordinate"},
"y": {"type": "number", "description": "Y coordinate"},
"unit": {
"type": "string",
"enum": ["mm", "inch"],
"default": "mm",
"description": "Unit for x/y (default mm)",
},
},
"required": ["x", "y"],
},
"diameter": {
"type": "number",
"description": "Hole diameter in millimeters",
"description": "Hole (drill) diameter in millimeters",
"minimum": 0.1,
},
"padDiameter": {
"type": "number",
"description": "Pad diameter in millimeters (defaults to diameter + 1mm). For NPTH this only affects the solder-mask opening, not copper.",
"minimum": 0.1,
},
"required": ["x", "y", "diameter"],
"plated": {
"type": "boolean",
"default": False,
"description": "True for plated through-hole (PTH) with copper pad; false (default) for NPTH (mask only).",
},
"footprintLibId": {
"type": "string",
"description": "Optional library:name FPID (e.g. 'MountingHole:MountingHole_3.2mm'). Defaults to MountingHole:MountingHole_<diameter>mm. A non-empty FPID is required for the footprint to be selectable in KiCad's GUI Move tool.",
},
},
"required": ["position", "diameter"],
},
},
{

190
tests/test_add_mounting_hole.py Normal file
View File

@@ -0,0 +1,190 @@
"""
Regression tests for BoardOutlineCommands.add_mounting_hole.
Covers two prior bugs:
1. Empty FPID
The footprint was created with no library:name id, producing
`(footprint "" ...)` in the .kicad_pcb. KiCad's GUI Move tool refuses to
select footprints with no library link, so users couldn't drag the
resulting MHs in the editor.
2. NPTH pad on copper layers
The pad was emitted with the default LSET (`*.Cu` + `*.Mask`) even when
`plated:false`. With `padDiameter > diameter` that produces phantom
copper annular rings on every Cu layer, which trigger DRC clearance
errors against neighbouring nets.
"""
import sys
from pathlib import Path
from unittest.mock import MagicMock
import pytest
sys.path.insert(0, str(Path(__file__).parent.parent / "python"))
import pcbnew # noqa: E402 — pcbnew is stubbed by conftest
@pytest.fixture
def fresh_pcbnew_mock(monkeypatch):
"""
The conftest pcbnew is a long-lived MagicMock. Reset its call history
before each test so we can make precise assertions about what
add_mounting_hole calls on the pcbnew API.
"""
pcbnew.reset_mock()
# PAD_ATTRIB constants must compare unequal so the conditional in the
# implementation picks the right branch.
pcbnew.PAD_ATTRIB_NPTH = "NPTH"
pcbnew.PAD_ATTRIB_PTH = "PTH"
pcbnew.PAD_SHAPE_CIRCLE = "circle"
pcbnew.F_Mask = "F.Mask"
pcbnew.B_Mask = "B.Mask"
return pcbnew
@pytest.fixture
def cmds(fresh_pcbnew_mock):
from commands.board.outline import BoardOutlineCommands
board = MagicMock(name="board")
board.GetFootprints.return_value = [] # no existing MHs
return BoardOutlineCommands(board=board)
def _captured_module(pcbnew_mock):
"""Return the FOOTPRINT mock instance created by the call under test."""
return pcbnew_mock.FOOTPRINT.return_value
def _captured_pad(pcbnew_mock):
"""Return the PAD mock instance created by the call under test."""
return pcbnew_mock.PAD.return_value
# ---------------------------------------------------------------------------
# Bug #1: empty FPID
# ---------------------------------------------------------------------------
class TestFootprintLibIdSet:
def test_default_fpid_uses_diameter(self, cmds, fresh_pcbnew_mock):
result = cmds.add_mounting_hole(
{
"position": {"x": 117, "y": 84.5, "unit": "mm"},
"diameter": 3.2,
"padDiameter": 3.5,
}
)
assert result["success"] is True
# LIB_ID was constructed with a non-empty library and footprint name
fresh_pcbnew_mock.LIB_ID.assert_called_once_with("MountingHole", "MountingHole_3.2mm")
# And the FOOTPRINT had its FPID set
_captured_module(fresh_pcbnew_mock).SetFPID.assert_called_once_with(
fresh_pcbnew_mock.LIB_ID.return_value
)
# The response surfaces the lib id used
assert result["mountingHole"]["footprintLibId"] == "MountingHole:MountingHole_3.2mm"
def test_default_fpid_strips_trailing_zeros(self, cmds, fresh_pcbnew_mock):
cmds.add_mounting_hole(
{
"position": {"x": 0, "y": 0, "unit": "mm"},
"diameter": 3.0, # would become "3.0mm" with %f, "3" with %g
}
)
# %g formatting: 3.0 → "3"
fresh_pcbnew_mock.LIB_ID.assert_called_once_with("MountingHole", "MountingHole_3mm")
def test_explicit_fpid_override(self, cmds, fresh_pcbnew_mock):
cmds.add_mounting_hole(
{
"position": {"x": 50, "y": 50, "unit": "mm"},
"diameter": 3.2,
"footprintLibId": "MountingHole:MountingHole_3.2mm_M3",
}
)
fresh_pcbnew_mock.LIB_ID.assert_called_once_with("MountingHole", "MountingHole_3.2mm_M3")
def test_explicit_fpid_without_colon_falls_back_to_mountinghole_lib(
self, cmds, fresh_pcbnew_mock
):
cmds.add_mounting_hole(
{
"position": {"x": 0, "y": 0, "unit": "mm"},
"diameter": 2.5,
"footprintLibId": "MyCustomHole",
}
)
fresh_pcbnew_mock.LIB_ID.assert_called_once_with("MountingHole", "MyCustomHole")
# ---------------------------------------------------------------------------
# Bug #2: NPTH pad layers
# ---------------------------------------------------------------------------
class TestNpthPadLayers:
def test_npth_pad_layers_are_mask_only(self, cmds, fresh_pcbnew_mock):
cmds.add_mounting_hole(
{
"position": {"x": 117, "y": 84.5, "unit": "mm"},
"diameter": 3.2,
"padDiameter": 3.5,
"plated": False,
}
)
pad = _captured_pad(fresh_pcbnew_mock)
# The pad must have been set to NPTH attr
pad.SetAttribute.assert_called_once_with("NPTH")
# SetLayerSet was called exactly once with an LSET that has
# F_Mask and B_Mask added — and nothing on Cu layers.
pad.SetLayerSet.assert_called_once()
lset_arg = pad.SetLayerSet.call_args.args[0]
added_layers = [c.args[0] for c in lset_arg.AddLayer.call_args_list]
assert "F.Mask" in added_layers
assert "B.Mask" in added_layers
assert all(
"Cu" not in str(layer) for layer in added_layers
), f"NPTH pad must not include any Cu layers, got: {added_layers}"
def test_npth_is_default(self, cmds, fresh_pcbnew_mock):
# Omit `plated` entirely; default must be NPTH.
cmds.add_mounting_hole(
{
"position": {"x": 0, "y": 0, "unit": "mm"},
"diameter": 3.2,
}
)
pad = _captured_pad(fresh_pcbnew_mock)
pad.SetAttribute.assert_called_once_with("NPTH")
pad.SetLayerSet.assert_called_once()
def test_pth_keeps_default_layers(self, cmds, fresh_pcbnew_mock):
cmds.add_mounting_hole(
{
"position": {"x": 0, "y": 0, "unit": "mm"},
"diameter": 3.2,
"padDiameter": 3.5,
"plated": True,
}
)
pad = _captured_pad(fresh_pcbnew_mock)
pad.SetAttribute.assert_called_once_with("PTH")
# For PTH, the default LSET (*.Cu + *.Mask) is correct, so we must
# NOT override it via SetLayerSet.
pad.SetLayerSet.assert_not_called()