How to reuse existing edge in combination with new geometry?

[wfraser]

Say I've got some solid with a complex shape, for example:

box = (
    cq.Workplane("XY")
    .box(10, 10, 1)
    .faces(">Z")
    .rect(3, 3, forConstruction=True)
    .vertices()
    .hole(1)
)

I want to use the outer edge combined with some other shape (say, a circle) and extrude that.

In this example the outer edge is just a square and I can easily just draw it again:

desiredShape = (
    box.faces(">Z")
    .rect(10, 10)
    .circle(4)
    .extrude(0.5, combine=False)
)

But what if it's actually a complex shape and I really don't want to re-define it?

I know how to select the outer edge, by finding the longest one:

box.faces(">Z").edges().sort(lambda edge: edge.Length() * -1).first()

but when I try to use that in place of the .rect(10, 10) in the previous block, it's seemingly ignored, and just extrudes the inner circle instead:

myShape = (
    box.faces(">Z")
    .edges()
    .sort(lambda edge: edge.Length()*-1)
    .first()
    .circle(4)
    .extrude(0.5, combine=False)
)

If I remove the call to .circle(), I get No pending wires present. I tried adding .toPending() which had no effect.

How do I reuse this existing edge in combination with other new geometry?

[lorenzncode]

Here are a few ideas. You were close with (1).

1. Solution with Workplane, toPending. Try selecting the wire not the edges:

# this matches the desired shape
myShape2 = (
    box.faces(">Z")
    .wires()
    .sort(lambda wire: wire.Length() * -1)
    .first()
    .toPending()
    .circle(4)
    .extrude(0.5, combine=False)
)

2. With Sketch. You can reuse the sketch for the original box and later for myShape.

import cadquery as cq

sk1 = cq.Sketch().rect(10, 10)
sk2 = sk1.copy().rarray(3, 3, 2, 2).circle(0.5, mode="s")

box1 = cq.Workplane().placeSketch(sk2).extrude(1)

# for comparison with myShape
desiredShape = box1.faces(">Z").rect(10, 10).circle(4).extrude(0.5, combine=False)

myShape = (
    box1.faces(">Z")
    .placeSketch(sk1.copy().circle(4, mode="s"))
    .extrude(0.5, combine=False)
)

3. With free func API.

import cadquery as cq
from cadquery.occ_impl.shapes import *

# name the box as box1 so it does not conflict with box() func
box1 = (
    cq.Workplane("XY")
    .box(10, 10, 1)
    .faces(">Z")
    .rect(3, 3, forConstruction=True)
    .vertices()
    .hole(1)
)

# for comparison with myShape
desiredShape = box1.faces(">Z").rect(10, 10).circle(4).extrude(0.5, combine=False)

wire1 = box1.faces(">Z").wires().sort(lambda wire: wire.Length() * -1).first().val()
wire2 = box1.faces(">Z").circle(4).val()  # new circle
face1 = face(wire1) - face(wire2)  # new face for desired shape
myShape = extrude(face1, (0, 0, 0.5))  # the desired shape

edit - remove issue link

[wfraser]

Ahh, thank you Lorenz! It seems I don't understand the distinction between edges and wires well enough yet. That was what I was missing.

[lorenzncode]

Regarding edges vs wires, see also the OCCT Introduction section for a description:
https://dev.opencascade.org/doc/overview/html/index.html#intro_overview_moddata

Edge – a shape corresponding to a curve and bounded by a vertex at each extremity;
Wire – a sequence of edges connected by their vertices;

Example build wire from edges:

from cadquery.occ_impl.shapes import segment, spline, wire

# create two edges
e1 = segment((0, 0), (10, 0))
e2 = spline([(10, 0), (0, 10)], [(1, 0), (0, -1)])

# create a wire
w1 = wire(e1, e2)

# create a wire with closing edge; three total edges
w2 = w1.close()