Circle cut🙏

[RickyIlBoss]

Good evening, I'm trying to understand if someone can kindly help me, on how to do this action on CadQuery as in the images I attached, this was done on Freecad.... but I want to show in the images... that it made a large circle and a smaller one... after creating them, and not extruded, it made something like two lines at 40°.... those it wants to keep, as you can see in the second final image, but I can't understand how to make two lines and make a cut and keep that part and make that cut and shape.... I can't understand how to do it.... split(keepTop or Bottom) doesn't work, but I don't know what other codes can be used to make this type of shape, which then made two lines and cut the circle, that is, two circles and put them together. I hope for an answer.... Thanks and good evening

[lorenzncode]

If I understand the question, here is an example using Sketch.

Create a ring.

from cadquery import Sketch

r = 75
ring = Sketch().circle(r).circle(r - 5, "s")

Create a pie shape slice.

pie = Sketch().arc((0, 0), r, -50, -80).segment((0, 0)).close().assemble()

Create the intersection.

result = ring * pie

[RickyIlBoss]

Good morning, thank you very much for the reply. I'll try the code later to study it, but one question: why did you use .arc? If in the image it showed that it created two lines? And then it cut that little piece? Why use the arc? Second question: why did you immediately recreate a new sketch after creating the first two circles and not re-recall it? Because otherwise a new sketch starts again... and it's different... thanks, I'm waiting for your reply.

[lorenzncode]

Why use the arc?

I started with a ring. To create the final shape I need another shape to perform the intersection. arc was an easy way to create the intersecting shape.

why did you immediately recreate a new sketch

Mostly to visualize and work on the shapes independently. You are right it can be combined into single sketch.:

r = 75
sk = (
    Sketch()
    .circle(r)
    .circle(r - 5, "s")
    .arc((0, 0), r, -50, -80)
    .segment((0, 0))
    .close()
    .assemble("i")
)

There are many solutions to create this shape. You can also create the shape directly from the 4 edges.:

r = 75
sk = (
    Sketch()
    .arc((0, 0), r, -50, -80)
    .segment(5, 50)
    .arc((0, 0), r - 5, 230, 80)
    .segment(5, -50)
    .assemble()
)

[RickyIlBoss]

Thank you so much for your reply. I'd like to ask you two more questions about things I don't understand, if that's okay with you. The first is about Sketch, which I don't understand. When I create a simple rectangle in cq.Sketch(), I don't really know how to go to a vertex or edge, fix myself there, and then move from there to make a circle. Because in Workplane, I place the vertex and use .workplane(centerOption="CenterOfMass") to fix myself there and move from there, but in Sketch, if I place the vertex, for example, and want to move from there—which I think the only way is with .push—and I enter a coordinate, it always starts from the center. But I'd like to go to that vertex, fix myself there, and move to make a circle. Like in Workplane, but I don't know how to do it in Sketch. I don't know what the code is, and I don't think there's anything complicated to write. Then, as a second question, about offset2D in Workplane. I'll post a YouTube video for a better understanding. When it gets to the top of the base rectangle, to construct a rectangle and perform a 2D offset with the filleted vertices, well, I know how to do it. It constructs the rectangle and automatically adds the filleted vertices, and then also automatically adds the 2D offset, which becomes smaller in proportion to the fillets' radius if the rectangle is much smaller than the original. When you choose the size, as you can see, as soon as you close the shape, you can extrude it like a frame, like making two circles in the Workplane, one large and one small, and automatically creates an empty hole inside. But there if I close and extrude it, it extrudes the entire solid of the smallest 2D offset I made, whole, but I asked some, and they told me that you have to create another internal one to make the border, but I don't understand if I make the large rectangle and make the smaller 2D offset that scales depending on the size you give it... of the smaller fillet that it does automatically in proportion, it is impossible to make the rectangle... make the 2D offset smaller than the fillet and smaller and make another internal one with a rectangle from scratch and recreate from scratch and know the same fillet that the 2D offset did automatically... so I wonder how it is possible to do, like the one in the video. Create the rectangle with the fillets at the vertices... make the smaller 2D offset. And extrude it as a border as done in the video??? Sorry the message is a bit long 😂 Thank you very much for your help and collaboration. Have a good evening

https://youtu.be/qt3TILp0QO4?si=N89oOHGlk32V6rTk

[lorenzncode]

When I create a simple rectangle in cq.Sketch(), I don't really know how to go to a vertex or edge, fix myself there, and then move from there to make a circle

import cadquery as cq

# circle centered on vertex
sk1 = cq.Sketch().rect(10, 20).vertices(">XY").circle(1)

# circle center offset from vertex
sk2 = (
    cq.Sketch().rect(10, 20).vertices(">X and <Y").map(lambda v: v.move(x=1)).circle(1)
)

Create the rectangle with the fillets at the vertices... make the smaller 2D offset. And extrude it as a border

Try Sketch, and placeSketch:

import cadquery as cq

sk = cq.Sketch().rect(25, 25).vertices().fillet(3).reset().wires().offset(-2, "s")

res = (
    cq.Workplane()
    .rect(200, 100)
    .extrude(10)
    .faces(">Z")
    .workplane()
    .pushPoints([(-60, 0), (60, 0)])
    .placeSketch(sk)
    .extrude(20)
)