"""Spur gear cut from the ISO 53 basic rack: module m, z teeth, pressure angle 20 degrees, addendum 1.0 m, dedendum 1.25 m, no profile shift, a plain disc
with a round bore. Axis along Z, centred on the origin. detail = "full": involute flanks, and below them the root curve the rack's tip corner cuts (a trochoid), which
undercuts small tooth counts as a real cutter does; flanks are smooth splines on computed involute points, the root curve a polyline. detail = "simple": a disc at the tip diameter, for big assemblies."""
import math

from steve import Model

module = 1  # ISO 54 module
teeth = 20  # Number of teeth
bore = 8  # mm Bore
width = 8  # mm Face width
detail = "full"  # full: real teeth; simple: a disc at the tip diameter

PRESSURE_ANGLE = 20  # degrees: ISO 53:1998 standard basic rack, profile A
ADDENDUM = 1.0  # x module: ISO 53
DEDENDUM = 1.25  # x module: ISO 53
FLANK_POINTS = 5  # involute points on each flank
MIN_WALL = 1.0  # x module: least ring left between the bore and the root circle, or the gear reads as a thin hoop

a = math.radians(PRESSURE_ANGLE)
rp = module * teeth / 2
rb = rp * math.cos(a)
ra = rp + ADDENDUM * module
h = DEDENDUM * module
rf = rp - h
if rf - bore / 2 < MIN_WALL * module:
    raise ValueError(f"Bore {bore} leaves less than one module of wall under the teeth: the root diameter is {2 * rf:.2f} mm.")


def involute(angle):
    return math.tan(angle) - angle


def flank_angle(r):
    """Half the tooth's angular width on the involute at radius r (r >= rb)."""
    return math.pi / (2 * teeth) + involute(a) - involute(math.acos(rb / r))


# the rack's tip corner, at c from the tooth's axis on the rack's tip line, traces the root curve as the rack rolls on the pitch circle
c = math.pi * module / 4 + h * math.tan(a)
start = c / rp
root_curve = []
for i in range(40):
    beta = start * (1 + i / 39 * 1.5)
    x = (c - beta * rp) * math.cos(beta) + rf * math.sin(beta)
    y = -(c - beta * rp) * math.sin(beta) + rf * math.cos(beta)
    root_curve.append((math.hypot(x, y), math.atan2(x, y)))
if h <= rp * math.sin(a) ** 2:   # no undercut: the involute starts where the rack's flank ends
    join = max(rf, math.sqrt(rb ** 2 + (rp * math.sin(a) - h / math.sin(a)) ** 2))
else:   # undercut: the root curve crosses the involute
    join = next((r for r, angle in root_curve if r >= rb and angle >= flank_angle(r)), max(rb, rf))
kept = [p for p in root_curve if p[0] < join - 1e-6]
step = max(1, len(kept) // 4)
root_part = kept[::step] + [(join, flank_angle(join) if join >= rb else kept[-1][1])] if kept else []
if root_part and join >= rb:
    root_part[-1] = (join, flank_angle(join))
flank_part = [(join + (ra - join) * i / (FLANK_POINTS - 1), 0) for i in range(FLANK_POINTS)]
flank_part = [(r, flank_angle(r)) for r, _ in flank_part]
if not root_part:
    root_part = [(rf, flank_angle(max(rf, rb)))]


def at(r, angle):
    return (r * math.sin(angle), r * math.cos(angle))


model = Model()
if detail == "simple":
    with model.sketch("gear_sketch", on="XY", name="Disc") as sk:
        sk.circle("tip", (0, 0), ra)
        sk.circle("bore_d", (0, 0), bore / 2)
else:
    with model.sketch("gear_sketch", on="XY", name="Tooth profile") as sk:
        for n in range(teeth):
            centre = 2 * math.pi * n / teeth
            rise = [at(r, centre - angle) for r, angle in root_part]
            fall = [at(r, centre + angle) for r, angle in reversed(root_part)]
            if len(rise) > 1:
                sk.polyline(f"root_a_{n}", rise, closed=False)
                sk.polyline(f"root_b_{n}", fall, closed=False)
            sk.spline(f"flank_a_{n}", [at(r, centre - angle) for r, angle in flank_part])
            sk.polyline(f"tip_{n}", [at(flank_part[-1][0], centre - flank_part[-1][1]), at(flank_part[-1][0], centre + flank_part[-1][1])], closed=False)
            sk.spline(f"flank_b_{n}", [at(r, centre + angle) for r, angle in reversed(flank_part)])
            following = centre + 2 * math.pi / teeth
            sk.polyline(f"land_{n}", [fall[-1], at(root_part[0][0], following - root_part[0][1])], closed=False)
        sk.circle("bore_d", (0, 0), bore / 2)
model.extrude("gear", "gear_sketch", distance=width, both=True, name="Gear")
model.material("steel-generic", color="#b4b8bd")
result = model.result()