134 lines
6.2 KiB
Python
134 lines
6.2 KiB
Python
"""Generate a small, real native KiCad board for integration tests.
|
|
|
|
Two passive two-pin headers, two distinct nets, two tracks and a ground zone.
|
|
No prior user design, test history, server path, or provider credential is used.
|
|
Run with KiCad's Python, not the web API virtual environment.
|
|
"""
|
|
import argparse
|
|
import json
|
|
from pathlib import Path
|
|
import uuid
|
|
|
|
|
|
def symbol_definition(library, name):
|
|
text = library.read_text()
|
|
start = text.index(f'(symbol "{name}"')
|
|
depth = 0
|
|
quoted = escaped = False
|
|
for end in range(start, len(text)):
|
|
char = text[end]
|
|
if escaped:
|
|
escaped = False
|
|
elif char == "\\" and quoted:
|
|
escaped = True
|
|
elif char == '"':
|
|
quoted = not quoted
|
|
elif not quoted:
|
|
if char == "(":
|
|
depth += 1
|
|
elif char == ")":
|
|
depth -= 1
|
|
if depth == 0:
|
|
return text[start:end + 1]
|
|
raise ValueError("Incomplete library symbol")
|
|
|
|
|
|
def make_project(directory, variant="good"):
|
|
import pcbnew as pcb
|
|
|
|
directory = Path(directory)
|
|
directory.mkdir(parents=True, exist_ok=False)
|
|
name = "native-smoke"
|
|
root_id = str(uuid.uuid4())
|
|
ids = [str(uuid.uuid4()), str(uuid.uuid4())]
|
|
fp_id = "Connector_PinHeader_2.54mm:PinHeader_1x02_P2.54mm_Vertical"
|
|
lib_id = "Connector_Generic:Conn_01x02"
|
|
definition = symbol_definition(Path("/usr/share/kicad/symbols/Connector_Generic.kicad_sym"), "Conn_01x02")
|
|
definition = definition.replace('(symbol "Conn_01x02"', f'(symbol "{lib_id}"', 1)
|
|
sch = [f'(kicad_sch (version 20250114) (generator "vibemake_kicad_test") (uuid "{root_id}") (paper "A4")',
|
|
f'(lib_symbols {definition})']
|
|
for index, sid in enumerate(ids):
|
|
ref = f"J{index + 1}"
|
|
x, y = 76.2 + 50.8 * index, 76.2
|
|
sch.append(f'''(symbol (lib_id "{lib_id}") (at {x} {y} 0) (unit 1)
|
|
(in_bom yes) (on_board yes) (dnp no) (uuid "{sid}")
|
|
(property "Reference" "{ref}" (at {x + 2.54} {y} 0) (effects (font (size 1.27 1.27)) (justify left)))
|
|
(property "Value" "Conn_01x02" (at {x + 2.54} {y + 2.54} 0) (effects (font (size 1.27 1.27)) (justify left)))
|
|
(property "Footprint" "{fp_id}" (at {x} {y} 0) (effects (font (size 1.27 1.27)) (hide yes)))
|
|
(instances (project "{name}" (path "/{root_id}" (reference "{ref}") (unit 1)))))''')
|
|
for pin, net in [(1, "VIN"), (2, "GND")]:
|
|
px, py = x - 5.08, y + 2.54 * (pin - 1)
|
|
lx = px - 7.62
|
|
sch.append(f'(wire (pts (xy {lx:.4f} {py:.4f}) (xy {px:.4f} {py:.4f})) (stroke (width 0) (type default)) (uuid "{uuid.uuid4()}"))')
|
|
sch.append(f'(label "{net}" (at {lx:.4f} {py:.4f} 0) (effects (font (size 1.27 1.27)) (justify left bottom)) (uuid "{uuid.uuid4()}"))')
|
|
sch.append('(embedded_fonts no))')
|
|
(directory / f"{name}.kicad_sch").write_text("\n".join(sch))
|
|
(directory / f"{name}.kicad_pro").write_text(json.dumps({"meta": {"filename": f"{name}.kicad_pro", "version": 1}}))
|
|
# Project-local tables make the example independent of first-run GUI setup.
|
|
(directory / "sym-lib-table").write_text('(sym_lib_table (version 7) (lib (name "Connector_Generic")(type "KiCad")(uri "/usr/share/kicad/symbols/Connector_Generic.kicad_sym")(options "")(descr "")))')
|
|
(directory / "fp-lib-table").write_text('(fp_lib_table (version 7) (lib (name "Connector_PinHeader_2.54mm")(type "KiCad")(uri "/usr/share/kicad/footprints/Connector_PinHeader_2.54mm.pretty")(options "")(descr "")))')
|
|
board = pcb.BOARD()
|
|
nets = {}
|
|
for name_net in ["VIN", "GND"]:
|
|
net = pcb.NETINFO_ITEM(board, "/" + name_net)
|
|
board.Add(net)
|
|
nets[name_net] = net
|
|
footprints = []
|
|
for index, sid in enumerate(ids):
|
|
fp = pcb.FootprintLoad("/usr/share/kicad/footprints/Connector_PinHeader_2.54mm.pretty", "PinHeader_1x02_P2.54mm_Vertical")
|
|
fp.SetFPIDAsString(fp_id)
|
|
fp.SetReference(f"J{index + 1}")
|
|
fp.SetValue("Conn_01x02")
|
|
path = pcb.KIID_PATH()
|
|
path.push_back(pcb.KIID(root_id))
|
|
path.push_back(pcb.KIID(sid))
|
|
fp.SetPath(path)
|
|
fp.SetPosition(pcb.VECTOR2I(pcb.FromMM(10 + 20 * index), pcb.FromMM(10)))
|
|
board.Add(fp)
|
|
for pad in fp.Pads():
|
|
pad.SetNet(nets["VIN" if pad.GetNumber() == "1" else "GND"])
|
|
footprints.append(fp)
|
|
for start, end in [((3, 3), (37, 3)), ((37, 3), (37, 24)), ((37, 24), (3, 24)), ((3, 24), (3, 3))]:
|
|
shape = pcb.PCB_SHAPE()
|
|
shape.SetShape(pcb.SHAPE_T_SEGMENT)
|
|
shape.SetLayer(pcb.Edge_Cuts)
|
|
shape.SetStart(pcb.VECTOR2I(*[pcb.FromMM(v) for v in start]))
|
|
shape.SetEnd(pcb.VECTOR2I(*[pcb.FromMM(v) for v in end]))
|
|
shape.SetWidth(pcb.FromMM(.05))
|
|
board.Add(shape)
|
|
for pin, net in [("1", "VIN"), ("2", "GND")]:
|
|
if variant == "unrouted" and pin == "1":
|
|
continue
|
|
pads = [next(p for p in fp.Pads() if p.GetNumber() == pin) for fp in footprints]
|
|
track = pcb.PCB_TRACK(board)
|
|
track.SetStart(pads[0].GetPosition())
|
|
track.SetEnd(pads[1].GetPosition())
|
|
track.SetWidth(pcb.FromMM(.6))
|
|
track.SetLayer(pcb.F_Cu)
|
|
track.SetNet(nets[net])
|
|
board.Add(track)
|
|
zone = pcb.ZONE(board)
|
|
zone.SetLayer(pcb.B_Cu)
|
|
zone.SetNet(nets["GND"])
|
|
zone.SetLocalClearance(pcb.FromMM(.25))
|
|
zone.SetThermalReliefGap(pcb.FromMM(.3))
|
|
zone.SetThermalReliefSpokeWidth(pcb.FromMM(.3))
|
|
zone.SetPadConnection(pcb.ZONE_CONNECTION_FULL)
|
|
zone.Outline().NewOutline()
|
|
for x, y in [(4, 4), (36, 4), (36, 23), (4, 23)]:
|
|
zone.Outline().Append(pcb.FromMM(x), pcb.FromMM(y))
|
|
board.Add(zone)
|
|
if variant == "wrong-net":
|
|
pad = next(p for p in footprints[1].Pads() if p.GetNumber() == "1")
|
|
pad.SetNet(nets["GND"])
|
|
pcb.SaveBoard(str(directory / "native-smoke.kicad_pcb"), board)
|
|
return directory / "native-smoke.kicad_pro"
|
|
|
|
|
|
if __name__ == "__main__":
|
|
parser = argparse.ArgumentParser()
|
|
parser.add_argument("directory")
|
|
parser.add_argument("--variant", choices=["good", "unrouted", "wrong-net"], default="good")
|
|
args = parser.parse_args()
|
|
print(make_project(args.directory, args.variant))
|