fix(add_mounting_hole): set FPID and restrict NPTH pad to mask layers (#154)
`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
@@ -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}",
|
||||
},
|
||||
}
|
||||
|
||||
|
||||
@@ -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,
|
||||
},
|
||||
"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": ["x", "y", "diameter"],
|
||||
"required": ["position", "diameter"],
|
||||
},
|
||||
},
|
||||
{
|
||||
|
||||
Reference in New Issue
Block a user