Twisted Part

[RickyIlBoss]

Good morning, I'm new to cadquery.... and I would like to know how to build this piece that I attached below.... how do you create it, because seeing in some videos on YouTube, they first create two separate pieces like I did and then connect the vertices or edges where the connection needs to be made and then click on the fusion curve from that I remember it was called that on freecad or other software..... on cadquery I don't know how to make this piece.... I tried to do twistExtrude but everything goes wrong.... I would like to first create the two pieces and the angle I want and then connect them like this piece that I attached..... I hope someone can explain it to me🙏 Thanks have a good day

[adam-urbanczyk]

It is definitely possible. Could you share your code first?

[RickyIlBoss]

import cadquery as cq

reslt=(
       cq.Workplane()
       .moveTo(0,10).radiusArc((0,-10),-10)
       .hLine(10).vLine(20).hLine(-10).close()
       .workplane().circle(10/2).extrude(4)
      )


result=(
        reslt.mirror("YZ").translate((44,0,0)).rotate((0,0,0),(1,0,0),90)
        )

This is my code, I just created the pieces as mentioned...but now I'm at the point of how to connect the lines to the vertices or edges as in the sketch. Thanks

[RickyIlBoss]

Good morning, did you receive the message with the code I sent you? I hope I didn't send it incorrectly. Thanks.

[RickyIlBoss]

It is definitely possible. Could you share your code first?

import cadquery as cq

reslt=(
cq.Workplane()
.moveTo(0,10).radiusArc((0,-10),-10)
.hLine(10).vLine(20).hLine(-10).close()
.workplane().circle(10/2).extrude(4)
)

result=(
reslt.mirror("YZ").translate((44,0,0)).rotate((0,0,0),(1,0,0),90)
)

This is my code, I just created the pieces as mentioned...but now I'm at the point of how to connect the lines to the vertices or edges as in the sketch. Thanks

[lorenzncode]

Here's my try using loft.

from cadquery import Sketch
from cadquery.func import *
from cadquery.vis import show

th = 4
sk1 = Sketch().rect(10, 20).moved(x=5).circle(10).clean().circle(5, "s")
fsk1 = sk1.faces().val().moved(z=-th / 2)
part1 = extrude(fsk1, (0, 0, th))
part2 = part1.mirror("YZ").moved(x=45, rx=-90)

f1 = part1.faces(">X")
f2 = part2.faces("<X")
f2 = Face(f2.wrapped.Reversed())

eps = 1e-3
twist = loft(
    f1.moved(x=-eps),
    f1,
    f2,
    f2.moved(x=eps),
    parametrization="chordal",
    compat=False,
)

result = part1 + twist + part2
show(result, width=500, height=500)

I'm not very familiar with the loft options so maybe there are better methods.

[adam-urbanczyk]

I think sweep with an aux spine is the canonical solution.

from cadquery import Sketch
from cadquery.func import *

# base parts creation
th = 4
sk1 = Sketch().rect(10, 20).moved(x=5).circle(10).clean().circle(5, "s")
fsk1 = sk1.faces().val().moved(z=-th / 2)
part1 = extrude(fsk1, (0, 0, th))
part2 = part1.mirror("YZ").moved(x=45, rx=-90)

# select faces to be connected
f1 = part1.faces(">X")
f2 = part2.faces("<X")
eps = 1e-3

# paths
tgts = [(1,0,0), (1,0,0)]
path = spline((f1.Center(), f2.Center()), tgts=tgts)
aux = spline((f1.Center() - Vector(0,eps,0), f2.Center() - Vector(0,0,eps)), tgts=tgts)

# twisted sweep
twist = sweep(f1, path, aux)

# combine everything
result = fuse(part1, twist, part2)

#%% and show
from cadquery.vis import show
show(result)

[lorenzncode]

Got it. Marking as answer.