Commander1024
c0f7a1ad51
- Add pinned STEP-derived DE-9 mechanical measurements and provenance - Refresh placement, routing, silkscreen, and nominal CAD envelopes - Document provisional dimensions, assumptions, and validation status
130 lines
6.7 KiB
Python
130 lines
6.7 KiB
Python
#!/usr/bin/env python3
|
|
"""Read-only PCB checks and fresh KiCad reports; does not regenerate or save PCB.
|
|
|
|
Requires KiCad's pcbnew binding in system Python. The known U2 footprint parity
|
|
warning is reported explicitly, not hidden or added to KiCad's exclusions.
|
|
"""
|
|
import hashlib
|
|
import json
|
|
from pathlib import Path
|
|
import subprocess
|
|
import xml.etree.ElementTree as ET
|
|
import pcbnew as p
|
|
|
|
ROOT=Path(__file__).resolve().parent
|
|
PCB=ROOT/"serial-carrier.kicad_pcb"
|
|
OUT=ROOT/"validation"
|
|
|
|
def run(*args):
|
|
subprocess.run(args,check=True,cwd=ROOT)
|
|
|
|
run("kicad-cli","sch","export","netlist","--format","kicadxml","-o",str(OUT/"pcb-source-netlist.xml"),str(ROOT/"serial-carrier.kicad_sch"))
|
|
run("kicad-cli","pcb","drc","--format","json","--all-track-errors","--severity-all","--schematic-parity","-o",str(OUT/"pcb-parity-drc.json"),str(PCB))
|
|
board=p.LoadBoard(str(PCB))
|
|
source=ET.parse(OUT/"pcb-source-netlist.xml").getroot()
|
|
comps={c.get("ref"):c for c in source.findall("components/comp")}
|
|
footprints={f.GetReference():f for f in board.GetFootprints()}
|
|
assert set(footprints)==set(comps)|{"H1","H2","H3","H4"}
|
|
assert board.GetCopperLayerCount()==2
|
|
assert p.ToMM(board.GetDesignSettings().GetBoardThickness())==1.6
|
|
outline=[d for d in board.GetDrawings() if d.GetLayer()==p.Edge_Cuts]
|
|
assert len(outline)==6
|
|
points={(round(p.ToMM(v.x)-100,5),round(p.ToMM(v.y)-100,5)) for d in outline for v in (d.GetStart(),d.GetEnd())}
|
|
expected_outline=[(36,0),(82,0),(82,80),(0,80),(0,19),(36,19)]
|
|
assert points==set(expected_outline)
|
|
expected_edges={frozenset((a,b)) for a,b in zip(expected_outline,expected_outline[1:]+expected_outline[:1])}
|
|
actual_edges={frozenset((round(p.ToMM(v.x)-100,5),round(p.ToMM(v.y)-100,5))
|
|
for v in (d.GetStart(),d.GetEnd())) for d in outline}
|
|
assert actual_edges==expected_edges
|
|
placements={"U1":(8,23),"U2":(43,26.670),"DS1":(43,36),
|
|
"R1":(43,34),"R2":(54,34),"R3":(65,34),
|
|
"SW1":(43,68),"SW2":(55,68),"SW3":(67,68),
|
|
"H1":(3.5,22.5),"H2":(3.5,75),"H3":(78,4),"H4":(78,76)}
|
|
for ref,(x,y) in placements.items():
|
|
position=footprints[ref].GetPosition()
|
|
assert position.x==p.FromMM(x+100) and position.y==p.FromMM(y+100),ref
|
|
assert footprints[ref].GetOrientationDegrees()==0,ref
|
|
assert len(board.Zones())==1
|
|
reserve=board.Zones()[0]
|
|
assert reserve.GetIsRuleArea() and reserve.IsOnLayer(p.F_Cu) and reserve.IsOnLayer(p.B_Cu)
|
|
assert reserve.GetDoNotAllowTracks() and reserve.GetDoNotAllowVias() and reserve.GetDoNotAllowZoneFills()
|
|
contour=reserve.Outline().COutline(0)
|
|
assert {(p.ToMM(contour.CPoint(i).x),p.ToMM(contour.CPoint(i).y)) for i in range(contour.PointCount())}=={(110,119),(131,119),(131,132),(110,132)}
|
|
# Reference bare-PCB front is 26.670 mm above the U2 pad-row origin.
|
|
u2_front=p.ToMM(footprints['U2'].GetPosition().y)-26.670
|
|
assert abs(u2_front-100)<1e-6
|
|
assert any(isinstance(g,p.PCB_SHAPE) and g.GetLayer()==p.F_Fab and
|
|
g.GetShape()==p.SHAPE_T_SEGMENT and
|
|
g.GetStart().y==p.FromMM(100) and g.GetEnd().y==p.FromMM(100)
|
|
for g in footprints['U2'].GraphicalItems()), 'U2 bare-PCB front not flush'
|
|
assert max(x for x,y in points)-min(x for x,y in points)==82
|
|
assert max(y for x,y in points)-min(y for x,y in points)==80
|
|
padnets={}
|
|
for net in source.findall("nets/net"):
|
|
for node in net.findall("node"):
|
|
padnets[(node.get("ref"),node.get("pin"))]=net.get("name")
|
|
seen=set()
|
|
for ref,comp in comps.items():
|
|
fp=footprints[ref]
|
|
assert fp.GetValue()==comp.findtext("value"),ref
|
|
assert fp.GetPath().AsString().endswith("/"+comp.findtext("tstamps")),ref
|
|
wanted=comp.findtext("footprint")
|
|
if ref=="U2":
|
|
assert not wanted
|
|
assert fp.GetFPIDAsString()=="Carrier:MAX3243_Reference_Provisional"
|
|
else:
|
|
assert fp.GetFPIDAsString()==wanted,ref
|
|
for pad in fp.Pads():
|
|
if not pad.GetNumber():
|
|
continue
|
|
key=ref,pad.GetNumber()
|
|
assert pad.GetNetname()==padnets[key],(key,pad.GetNetname(),padnets[key])
|
|
seen.add(key)
|
|
assert seen==set(padnets),"Missing or extra electrical pads"
|
|
for ref in ("H1","H2","H3","H4"):
|
|
assert footprints[ref].IsBoardOnly()
|
|
pads=list(footprints[ref].Pads())
|
|
assert len(pads)==1 and pads[0].GetDrillSize().x==p.FromMM(3.2)
|
|
assert pads[0].GetAttribute()==p.PAD_ATTRIB_NPTH
|
|
tracks=list(board.GetTracks())
|
|
assert tracks,"Draft unexpectedly unrouted"
|
|
for track in tracks:
|
|
if isinstance(track,p.PCB_VIA):
|
|
assert track.GetDrillValue()==p.FromMM(0.3)
|
|
assert track.GetWidth(p.F_Cu)==p.FromMM(0.7)
|
|
else:
|
|
assert track.GetLayer() in (p.F_Cu,p.B_Cu)
|
|
expected=0.5 if track.GetNetname() in ("/+3V3","/GND") else 0.25
|
|
assert track.GetWidth()==p.FromMM(expected)
|
|
report=json.loads((OUT/"pcb-parity-drc.json").read_text())
|
|
assert not report["violations"],report["violations"]
|
|
assert not report["unconnected_items"],report["unconnected_items"]
|
|
parity=report["schematic_parity"]
|
|
assert len(parity)==1 and parity[0]["type"]=="footprint_symbol_mismatch",parity
|
|
assert len(parity[0]["items"])==1 and parity[0]["items"][0]["uuid"]==footprints["U2"].m_Uuid.AsString()
|
|
summary={
|
|
"carrier_bounds_mm":[82,80],
|
|
"outline_local_mm":expected_outline,
|
|
"placements_local_mm":placements,
|
|
"rf_reserve_absolute_mm":[110,119,131,132],
|
|
"u2_bare_pcb_front_local_y_mm":round(u2_front-100,6),
|
|
"nominal_user_confirmed_rs232_metal_mm":{"shell_overhang":3.870,"hex_mouth_overhang":2.870,"flange_front_inset":1.930},
|
|
"tracks":sum(not isinstance(t,p.PCB_VIA) for t in tracks),
|
|
"vias":sum(isinstance(t,p.PCB_VIA) for t in tracks),
|
|
"copper_layers":2,
|
|
"draft_thickness_mm":1.6,
|
|
"electrical_footprints":len(comps),
|
|
"proposed_M3_mounts":4,
|
|
"physical_DRC_violations":0,
|
|
"unconnected_items":0,
|
|
"schematic_pad_nets_match":True,
|
|
"known_parity_warning":"U2 reference footprint assigned on PCB only; schematic footprint intentionally blank; nominal male external metal dimensions user-confirmed",
|
|
"project_settings_sha256":hashlib.sha256((ROOT/'serial-carrier.kicad_pro').read_bytes()).hexdigest(),
|
|
"ignored_DRC_checks":report["ignored_checks"],
|
|
"not_validated":["male module pin map/header fit", "ESP32 geometry and complete assembly envelope/heights", "header/socket fit", "RF performance and antenna clearance", "power/return-path integrity", "USB power path", "OLED pull-ups", "fabrication process", "hardware operation"],
|
|
}
|
|
(OUT/"pcb-validation-summary.json").write_text(json.dumps(summary,indent=2)+"\n")
|
|
print("PCB draft verified: 82 x 80 mm; 2 copper layers; 0 physical DRC violations; 0 unrouted.")
|
|
print("All schematic pad nets match. One expected U2 footprint parity warning remains visible.")
|
|
print("Not fabrication-ready; see pcb-draft-notes.md and ignored checks in the DRC report.")
|