Selecting edges of swept object and filleting

[Ssw]

I'm trying to select faces on Z axis and then fillet edges, but |Z filter returns no faces despite >Z and <Z called separate return one face (one returns top and second bottom). Any advice on how to do it properly? 

Second thing is I want to perform multisection sweep to have different thickness where ellipse is wider. How can I do such sweep? I tried to supply rectangles with different heights but ended up with errors only.

Thanks in advance.

import cadquery as cq

import ocp_vscode as ov

radius = 23

result = cq.Workplane("XY").ellipse(radius, radius + 3)

result = (

cq.Workplane("YZ")

.center(-radius, 0)

.rect(2, 10)

.sweep(result)

)

# result = result.faces("|Z")

ov.show(result)

[Lorenz]

>  |Z filter returns no faces

Yes, although the result appears to contain planar faces, all of the faces are of type BSPLINE.  The "|Z" ParallelDirSelector does not work with this type of face currently.

You might workaround it by using LengthNthSelector or other selector:

# to select the inner edges on both top and bottom for fillet:
e_inner = result.edges(cq.selectors.LengthNthSelector(2))
# outer edges
e_outer = result.edges(cq.selectors.LengthNthSelector(3))
# outer top edge
e_outer_top = e_outer.edges(">>Z")

[Lorenz]

Try something like this for the sweep (CQ master):

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

radius = 23
path = cq.Workplane("XY").ellipse(radius, radius + 3)

# create profiles
prof1 = cq.Workplane("YZ").center(-radius, 0).rect(2, 10)
prof2 = cq.Workplane("YZ").center(radius, 0).rect(5, 10)

result = sweep([prof1.val(), prof2.val()], path.val(), True)

or with CQ2.4 :

result = (
    cq.Workplane()
    .add([prof1.val(), prof2.val()])
    .toPending()
    .sweep(path, multisection=True)
)

[Ssw]

Hi Lorenz,

thank you for your help. I checked your tips and came out with the results below. Unfortunately, fillet throws a mysterious error (to me of course ;)), looks like it does not work when thickness is different - in your example it works but only when swept rect has the same size. I spent some time today and was able to get the same shape as below script produces (my implementation was far more messy). How can I make the result symmetric in both X and Y axes?

import cadquery as cq

import ocp_vscode as ov

import cqkit as ck

radius = 23

radius2 = radius + 3

path = cq.Workplane("XY").ellipse(radius, radius2)

# create profiles

prof1 = cq.Workplane("YZ").center(-radius2, 0).rect(2, 10)

prof2 = cq.Workplane("XZ").center(-radius, 0).rect(1, 10)

prof3 = cq.Workplane("YZ").center(radius2, 0).rect(2, 10)

prof4 = cq.Workplane("XZ").center(radius, 0).rect(1, 10)

profs = [

prof1.val(),

prof2.val(),

prof3.val(),

prof4.val(),

]

result = (

cq.Workplane().add(profs)

.toPending()

.sweep(path, multisection=True)

)

# result = result.edges(cq.selectors.LengthNthSelector(2)).fillet(0.1)

ck.pprint_obj(result)

ov.show(result)

[Lorenz]

> How can I make the result symmetric in both X and Y axes?

Here is one method by creating an arc then mirroring the result.

import cadquery as cq

radius = 23
radius2 = radius + 3

# create ellipse arc path
path = cq.Workplane("XY").ellipseArc(radius, radius2, 0, 90).translate((radius, 0, 0))

# postions on path - where to create profiles
# 0 is start, 1 is end of path; add other pos as needed
ds = [0, 0.5, 1]
# width of profile at position index (height fixed at 10 below)
w_prof = [5, 2, 5]

# list of position and tangent vectors to define profile plane
positions = path.val().positions(ds)
tangents = [path.val().tangentAt(d) for d in ds]

# create the profiles
profs = []
for p, t, w in zip(positions, tangents, w_prof):
    plane1 = cq.Plane(origin=p, normal=t)
    wire1 = cq.Workplane(plane1).rect(w, 10)
    profs.append(wire1.val())

# for visualization of all profiles only
vis_profs = cq.Workplane().add(profs)

# create ring shape with multisection sweep
result_sweep = (
    cq.Workplane()
    .add(profs)
    .toPending()
    .sweep(path.val(), multisection=True)
    .mirror("XZ", union=True)
    .mirror("YZ", union=True)
)

# example fillet inside edges
result_sweep2 = (
    result_sweep.faces("|Z").edges(cq.selectors.LengthNthSelector(0)).fillet(0.2)
)

# example fillet top both edges
result_sweep3 = result_sweep.faces(">>Z").edges().fillet(0.2)

# compare with loft
result_loft = (
    cq.Workplane()
    .add(profs)
    .toPending()
    .loft()
    # .loft(True)  # also compare with ruled
    .mirror("XZ", union=True)
    .mirror("YZ", union=True)
)



Another example with Sketch:

import cadquery as cq

radius = 23
radius2 = radius + 3

th = 4  # thickness of ring

# ellipse ring
sk1 = cq.Sketch().ellipse(radius, radius2)
sk2 = cq.Sketch().ellipse(radius + th, radius2 + th)

# example: distribute shape along edge; replace mode
sk3 = sk1.copy().edges().distribute(8, 0, 1).circle(4, mode="r").reset()
# call reset when done with sketch selection

# combine sketches, extrude
result = cq.Workplane().placeSketch(sk2 - sk1 + sk3).extrude(10)
result = result.faces(">>Z").edges().fillet(0.2)

[Ssw]

I managed to get the required shape on my own; however, I have one more question. Which version of CadQuery are you using? I have 2.4.0, and I'm unable to run the second example. There are no addition and subtraction operators for sketches, and there is no "r" mode for Sketch.circle() method.

[Lorenz]

Sorry, I was using the master branch.  The example used several new Sketch features.