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).

python/commands/board/outline.py

@@ -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}",
                 },
             }