Cutting a cylinder with helix sweep result in "Compound is empty"

[realfun]

Hi I am trying to create an auger-shaped marble run lift with the following code, but when running it with latest cadquery it always yield an error: ValueError: Compound is empty

The code:

import cadquery as cq
from ocp_vscode import *

r = 18 # Radius of the helix
p = 18 # Pitch of the helix
h = 30 # Height of the helix

wire = cq.Wire.makeHelix(pitch=p, height=h, radius=r)
helix = cq.Workplane(obj=wire)
marble_track = (
    cq.Workplane('XZ')
    .center(r, 0)
    .circle(8)
    .sweep(helix)
)

post = cq.Workplane().cylinder(h, 22)

result = post.cut(marble_track)

show(result)

I visually inspected the marble_track & the post individually, they seem to be correct, but don't know why cutting the marble_track from the post would return empty compound.

I tried to cut the other way around to figure out what's going on, I.E. result = marble_track.cut(post), this time it yields something really weird.

After getting some help from anderson.pa in discord #general channel, change the post to be z-flush would make it render: post = cq.Workplane().cylinder(h, 22, centered=(True, True, False)), but change wire to a bigger height or change the post to smaller radius(18) would cause it to fail.

So it seems to be a bug particular to the helix sweep.

[lorenzncode]

I find the cut is successful for a range of rotation angles of the post cylinder around its center.

fail: 0 to ~79 success: ~80 to 360

import cadquery as cq
from cadquery.vis import show

r = 18  # Radius of the helix
p = 18  # Pitch of the helix
h = 30  # Height of the helix

wire = cq.Wire.makeHelix(pitch=p, height=h, radius=r)
helix = cq.Workplane(obj=wire)
marble_track = (
    cq.Workplane('XZ')
    .center(r, 0)
    .circle(8)
    .sweep(helix)
)

post = cq.Workplane().cylinder(h, 22).rotateAboutCenter((0, 0, 1), 80)

result = post.cut(marble_track)

show(result)

Of course I'd rather not consider the rotation of the cylinder in order for a successful cut. It appears to be an OCCT CAD kernel issue.

[realfun]

Thanks for looking into this! Curious how do you ever think of trying rotateAboutCenter? This never crossed my mind.

Indeed it works after rotateAboutCenter 80, though it breaks again if h is 31, giving no error and just a cylinder without the coil cut. But if the cylinder is created Z-flush with centered=(1, 1, 0), then it starts working again! Weird, and cumbersome, but it works now. Really appreciated the help. Here is the updated code as a successful work around.

import cadquery as cq
from ocp_vscode import *

r = 18  # Radius of the helix
p = 18  # Pitch of the helix
h = 200  # Height of the helix

wire = cq.Wire.makeHelix(pitch=p, height=h, radius=r)
helix = cq.Workplane(obj=wire)
marble_track = (
    cq.Workplane('XZ')
    .center(r, 0)
    .circle(8)
    .sweep(helix)
)

post = cq.Workplane().cylinder(h, 22, centered=(1, 1, 0)).rotateAboutCenter((0, 0, 1), 80)
result = post.cut(marble_track)

show(result)

I noticed there are some weird line every several rounds:

[lorenzncode]

Curious how do you ever think of trying rotateAboutCenter?

The boundary representation (BREP) of the cylinder includes a seam. The cylinder is not only defined by its origin, radius, height at the kernel level so I experimented with rotation to see if it affected the result.

Take a circle for example. https://dev.opencascade.org/doc/refman/html/classgp___circ.html "Describes a circle in 3D space. A circle is defined by its radius and positioned in space with a coordinate system"

The resulting edge or wire contains a vertex as shown here depending on the defined coordinate system.

import cadquery as cq
from cadquery.vis import show

circle = cq.Workplane().circle(10)
# mark the vertex
mark = cq.Workplane(origin=circle.vertices().val().Center()).sphere(1.0)

show(circle, mark)

though it breaks again if h is 31

Yes, modifying h or centered changes the problem and I find I had to play with the angle again (89 to 360 in case of h=31).

there are some weird line every several rounds:

That is from the intersection of the seam of the marble_track. See here:

[realfun]

Thanks for the detailed explaination, today I learnt :)

For anyone who searched to here, notice that in the original code a vertical circle is used to create the coil sweep, which is slightly off. To be truly perpendicular, it needs to be in a special angle that has to do with pitch and radius, updated code below:

import cadquery as cq
from ocp_vscode import *
from math import pi, atan, degrees

r = 18  # Radius of the helix
p = 18  # Pitch of the helix
h = 200  # Height of the helix

wire = cq.Wire.makeHelix(pitch=p, height=h, radius=r)
helix = cq.Workplane(obj=wire)
c = p / (pi * 2)
angle = -degrees(atan(r/c))  # Helix starting angle, with help of Wolfram Alpha
# print(angle)
marble_track = (
    cq.Workplane()
    .center(r, 0)
    .transformed(rotate=(angle, 0, 0))
    .circle(8)
    .sweep(helix)
)

post = cq.Workplane().cylinder(h, 22, centered=(1, 1, 0)).rotateAboutCenter((0, 0, 1), 80)
result = post.cut(marble_track)

show(result)