Modeling bend in face with slot

[lorenzncode]

The solution of #1996 does not preserve the slot. It looks like a different approach is needed to create a bend given a face with features such as slot/holes.

from cadquery import Sketch

sk1 = Sketch().rect(40, 20).push([(-10, 0)]).slot(10, 1, 0, "s").reset()

BEND_RADIUS = 1
THICKNESS = 1

# todo:
# - create bend at x=-10, around y, say -90 degrees
# - thicken/offset to given thickness 

[adam-urbanczyk]

I think the best angle of attack here would be to use edgeOn and map the original sketch onto the parametric space of the bent plate.

[nazeeh111]

Building on @adam-urbanczyk's UV-mapping suggestion, faceOn maps the outer boundary and all inner wires. For this sketch, split the flat face into two flanges and the bend strip, map only that strip, then sew and thicken the faces together. That keeps the slot across the bend.

Here is a CadQuery 2.8.0 example, with lengths in millimeters. inner_radius=1 is the inside radius; thickness is 1. The flat coordinates are treated as developed midsurface coordinates, with the bend zone centered at x=-10. Its length is pi * (inner_radius + thickness/2) / 2. The left flange stays in the XY plane; the right flange rotates -90° about +Y, toward +Z. The cylinder axis is parallel to Y through (start, 0, radius), or approximately (-11.178097, 0, 1.5) for these defaults. Thickness is symmetric about the midsurface.

from math import pi

import cadquery as cq
from cadquery.func import faceOn, offset, shell


def bent_slot(inner_radius=1.0, thickness=1.0, samples=50):
    # The original flat coordinates are developed midsurface coordinates.
    radius = inner_radius + thickness / 2
    start = -10 - pi * radius / 4
    end = -10 + pi * radius / 4
    sketch = cq.Sketch().rect(40, 20).push([(-10, 0)]).slot(10, 1, 0, "s").reset()
    flat = sketch.val()

    def strip(a, b):
        boundary = cq.Workplane().center((a + b) / 2, 0).rect(b - a, 20).val()
        return flat.intersect(cq.Face.makeFromWires(boundary))

    left, bend, right = strip(-20, start), strip(start, end), strip(end, 20)
    cylinder = cq.Solid.makeCylinder(radius, 20, pnt=(0, 0, -10))
    base = next(f for f in cylinder.Faces() if f.geomType() == "CYLINDER")
    base = (
        base.rotate((0, 0, 0), (0, 0, 1), -90)
        .rotate((0, 0, 0), (1, 0, 0), 90)
        .translate((start, 0, radius))
    )
    # Cylinder u is an angle; v runs along its axis. Map all boundary wires.
    uv = bend.transformGeometry(cq.Matrix([
        [1 / radius, 0, 0, -start / radius],
        [0, -1, 0, 10],
        [0, 0, 1, 0],
        [0, 0, 0, 1],
    ]))
    bend = faceOn(base, uv, N=samples, tol=1e-7)
    right = (
        right.translate((-end, 0, 0))
        .rotate((0, 0, 0), (0, 1, 0), -90)
        .translate((start + radius, 0, radius))
    )
    midsurface = shell(left, bend, right, tol=1e-6)
    return offset(midsurface, thickness / 2, both=True, cap=True, tol=1e-6)


result = bent_slot()
assert result.isValid() and len(result.Solids()) == 1
# In CQ-editor or another viewer: show_object(result)

faceOn uses curve interpolation; this uses 50 samples per mapped edge and a 1e-7 mapping tolerance, with 1e-6 sewing/thickening tolerances. The slot's rounded ends remain in the flat flanges in these dimensions. In Sketch.slot(10, 1), the straight span is 10, so the overall slot length is 11.

Checked with CadQuery 2.8.0 / OCCT 7.9.3: one valid solid, volume about 789.21461 mm³, and material/empty-space probes through the slot, adjacent plate and both bend seams. A fresh-process STEP readback retained the valid solid and open slot. Radius/thickness pairs (2, 0.8) and (0.5, 0.5) also produced one valid solid and passed volume and slot probes. This is a geometric construction; material bend allowance, neutral-axis shift and springback are separate.