Trouble with extrude

[Schmavery]

Using cq-editor v0.2.0 (and later cadquery==2.2.0b2 and cadquery-server==0.4.1)

I've been having a lot of fun playing with cadquery and but have unfortunately been running into some behaviors I can't explain. Not sure if these are me misunderstanding the tool or actual bugs.

I'm trying to build design an adapter for my vacuum hose which has a little clip on the side to secure it (The hose has a arm that hooks onto the wedge on the adapter). I was running into issues building it, and then tried to create a minimal example. The full code for what I was originally trying to build is included at the bottom.

Bug 1:

result = (
  cq.Workplane("XY").circle(5).extrude(5, both=True).faces("<Z")
    .workplane().union(cq.Workplane("XY").box(5, 5, 5).translate((10, 0, 0)))  # not sure how best to do this without the union
    .faces("-X").wires().toPending().extrude(5)
)

(Also reducing the extrude amount to be below 5 gives Null TopoDS_Shape object error.. not sure why). Increasing the amount makes the box longer but not thicker.

Bug 2:
I converted this to use another workplane instead of the wires and for some reason got the same result until I used centerOption="CenterOfMass". I then "shelled" the cylinder since that was causing a problem in the original code.

Sure enough, .extrude(1) worked fine, but .extrude(2) actually crashed cq-editor! I then switched to using cadquery==2.2.0b2 and cadquery-server==0.4.1 in vscode to see if it would help.

With the new version of cadquery, the code below no longer crashes but the box disappears, showing only the hollow cylinder.

result = (
  cq.Workplane("XY").circle(5).extrude(5, both=True)
    .faces("|Z").shell(1)
    .faces("<Z").workplane().union(cq.Workplane("XY").box(5, 5, 5).translate((10, 0, 0)))
    .faces("-X").workplane(centerOption="CenterOfMass").rect(5, 5).extrude(2) # <- This extrude is behaving weird
)

Bug 3:
What I would ideally like is to just extrude the rect until it hits the side of the hollow tube, but the "next" option to extrude doesn't do what I would expect either. Why is it going all the way through the cylinder to the other side?

result = (
  cq.Workplane("XY").circle(5).extrude(5, both=True)
    .faces("|Z").shell(1)
    .faces("<Z").workplane().union(cq.Workplane("XY").box(5, 5, 5).translate((10, 0, 0)))
    .faces("-X").workplane(centerOption="CenterOfMass").rect(5, 5).extrude("next")
)

Original code:
I've included my original attempt (cadquery==2.2.0b2 cadquery-server==0.4.1) here in case it helps with context and/or in case anyone has any suggestions on how I could write it better.

portOD = 80
portID = 75
hoseOD = 50
wallThickness = 4
portLength = 40
hoseLength = 40
portClipHeight = 10
transitionLength = 30
clearance = 0.5

hoseClipOffset = 5
hoseClipDepth = 4
hoseClipWidth = 20
numClipWedges = 5

hoseClipHeight = hoseClipDepth*numClipWedges

clip = (cq.Workplane().tag("clip")
    .pushPoints([((hoseClipDepth)*i - (hoseClipHeight/2) + (hoseClipDepth/2), 0) for i in range(numClipWedges)])
    .wedge(dx=hoseClipDepth, dy=hoseClipDepth, dz=hoseClipWidth, xmin=0, zmin=0, xmax=0, zmax=hoseClipWidth, centered=True)
)

result = (cq.Workplane("XY")
    .circle(hoseOD/2 - clearance).extrude(hoseLength)
    .faces(">Z").wires().toPending()
    .workplane(offset=transitionLength)
    .circle(portOD/2 + wallThickness + clearance).loft(combine=True)
    .faces(">Z").wires().toPending().extrude(portLength)
    .faces("|Z").shell(wallThickness)
    .faces("<Z").workplane()
    .union(clip.rotate((0, 0, 0), (1, 0, 0), 90).rotate((0, 0, 0), (0, 1, 0), 90).translate((hoseOD/2+hoseClipDepth + hoseClipOffset, 0, hoseClipHeight/2)))
    .faces("-X").workplane(centerOption="CenterOfMass").rect(hoseClipHeight, hoseClipWidth).extrude("next")
)

Thank you!

[lorenzncode]

1. If I understand correctly, the box represents the clip in the full example code. You would like to extrude from the flat face of the clip part to the cylinder.

   In this example, your intended extrude direction is -X, however the actual extrude is in -Z due to the workplane created after faces("<Z").

2. and 3. appear to be issues with shell and/or extrude("next")? As a workaround, here is variation using revolve and then project, and loft to create the joined part.

import cadquery as cq
from cadquery.selectors import BoxSelector, AreaNthSelector

portOD = 80
hoseOD = 50
wallThickness = 4
portLength = 40
hoseLength = 40
transitionLength = 30
clearance = 0.5
hoseClipOffset = 5
hoseClipDepth = 4
hoseClipWidth = 20
numClipWedges = 5

hoseClipHeight = hoseClipDepth * numClipWedges

s_clip = (
    cq.Sketch()
    .push([(-hoseClipDepth / 2, -hoseClipDepth / 2)])  # to center
    .rarray(hoseClipDepth, hoseClipDepth, 1, numClipWedges)
    .segment((0, 0), (0.1, 0))  # to have clean face
    .segment((0.1, 0), (hoseClipDepth, hoseClipDepth))
    .segment((0, hoseClipDepth))
    .close()
    .assemble()
)

clip = cq.Workplane("XZ").placeSketch(s_clip).extrude(hoseClipWidth / 2, both=True)

clip = (
    clip.translate(
        (hoseOD / 2 + hoseClipDepth + hoseClipOffset, 0, hoseClipHeight / 2 + 5)
    )
    .solids()
    .tag("clip")
    .faces("<X")
    .tag("xface")
)

# points on the inside of the adapter
pts = [
    (hoseOD / 2 - clearance, 0),
    (hoseOD / 2 - clearance, hoseLength),
    (portOD / 2 + wallThickness + clearance, hoseLength + transitionLength),
    (
        portOD / 2 + wallThickness + clearance,
        hoseLength + transitionLength + portLength,
    ),
]

# add outside points and close
pts.extend([(p[0] + wallThickness, p[1]) for p in reversed(pts)])
pts.append(pts[0])

result = cq.Workplane("XZ").sketch().polygon(pts).finalize().revolve()

# Box selector returns two faces (from hose portion)
# Area selector 0 = inner, 1 outer
face_adapter = result.faces(
    BoxSelector(
        (-hoseOD / 2 - wallThickness, -hoseOD / 2 - wallThickness, 0.1),
        (hoseOD / 2 + wallThickness, hoseOD / 2 + wallThickness, hoseLength - 0.1),
    )
).faces(AreaNthSelector(1))

face_project = clip.val().project(face_adapter.val(), (-1, 0, 0))

join = cq.Solid.makeLoft(
    [clip.faces(tag="xface").val().Wires()[0], face_project.Wires()[0]]
)

result = result.union(join).union(clip.solids(tag="clip"))