How to construct a sketch using the edga-based API and then extrude it in a empty workplane.

[Willy-Schnackenpfefferhausen]

I checked CadQuery's read the docs (https://cadquery.readthedocs.io) for working with sketches. Perhaps I missed something, but I would like to extrude a sketch to get my first 3D object. From the examples I see how to add a sketch to an existing face, however I am running into road blocks when trying to extrude a sketch off the default workplane.

Here is my example sketch:

    r1 = 3/16
    r2 = 2*r1
    h = 2
    b = 1
    angle = 30 # degrees

    result = (
        cq.Sketch()
        .segment((0,0),(0,h))
        .segment(r1,0)
        .segment(h,-90)
        .arc((r2,0), r1, 180, angle)
        .segment(b, 270+angle)
        .segment(r1,180+angle)
        .segment(b,90+angle)
        .arc((r2,0), r2, 180+angle, -angle)
        .close()
    )

I have tried a several things so far including:

   result = (
        cq.Workplane("XY")
        .sketch()
...
        .extrude(10)
    )

This leads to the error 'Sketch; object has no attribute 'extrude'. Since the workplane does not yet have a face, I cannot use .faces('>Z') to build my sketch. I also tried .placeSketch(result), but I hit a similar error. I see that one can transform a workplane. Nevertheless sketching seems to require a face or something concrete to build off in order to extrude.

I would be grateful for guidance.

[jmwright]

Here's an example I have in my notes that seems to work.

import cadquery as cq

s1 = (
    cq.Sketch()
    .rect(30, 40)
    .rect(10, 10, mode="s", tag="rectcut")
    .vertices(">X", tag="rectcut")
    .fillet(1)
    .vertices("<X", tag="rectcut")
    .fillet(2)
)

r = cq.Workplane().placeSketch(s1).extrude(10)

[Willy-Schnackenpfefferhausen]

Thank you for the quick reply. I tried something similar in my own attempts, which after testing your solution to my sketch, leads to ValueError: No pending wires present. To summarize @lorenzncode's explanation as to why it resulted in a ValueError: The call to .rect(...) constructs a face. My sketch does not create a face.

[lorenzncode]

Remove close() (because the final arc already closes the edges).
Add assemble().

import cadquery as cq

r1 = 3/16
r2 = 2*r1
h = 2
b = 1
angle = 30 # degrees

s = (
    cq.Sketch()
    .segment((0,0),(0,h))
    .segment(r1,0)
    .segment(h,-90)
    .arc((r2,0), r1, 180, angle)
    .segment(b, 270+angle)
    .segment(r1,180+angle)
    .segment(b,90+angle)
    .arc((r2,0), r2, 180+angle, -angle)
    .assemble()
)

result = cq.Workplane().placeSketch(s).extrude(10)

See the docs section on the Edge-based API and the notes on assemble.
https://cadquery.readthedocs.io/en/latest/sketch.html#edge-based-api

assemble is not required in @jmwright's example because it calls rect which automatically results in constructing a face (face-based API).

To define the sketch inline (instead of placeSketch):

...

result  = (
    cq.Workplane()
    .sketch()
    .segment((0,0),(0,h))
    ...
    .arc((r2,0), r2, 180+angle, -angle)
    .assemble()
    .finalize() # finish the sketch
    .extrude(10)
)

[Willy-Schnackenpfefferhausen]

I tested both solutions (Using placeSketch(s) & inline). Both were successful. Thank you!

Also, I appreciate your advice on assemble. To quote https://cadquery.readthedocs.io/en/latest/sketch.html#edge-based-api "Once the construction is finished it has to be converted to the face-based representation using assemble(). Afterwards, face based operations can be applied."

Thank you also for the fast reply.

[adam-urbanczyk]

@Willy-Schnackenpfefferhausen also read this section of the docs https://cadquery.readthedocs.io/en/latest/sketch.html#workplane-integration .

[Willy-Schnackenpfefferhausen]

Thank you for the suggestion.

In each of the cases that are presented in #workplane-integration, the code begins with an existing face. I began by using these examples but unfortunately overlooked the answer to my question, which was addressed in #edge-based-api on the same page. The necessary step for my situation was to use assemble().

[adam-urbanczyk]

AFAICT your question was about beginning with a sketch, not rly about assemble. If this is not correct maybe amend the title.

[Willy-Schnackenpfefferhausen]

I see from the solution how the title comes into question, because I would have had the same issues trying to extrude this sketch on an existing face. I did not know that at the time of asking.

The solution did answer my initial question as well, which is how does one begin a model with a sketch. That is without:

cq.Workplane()
.box(5,5,1)
.faces('>Z')

From the examples in #workplane-integration I could not find how I could build off an empty workplane. Each example used .faces(...).

Based on this, what would you propose I change my title to?

[adam-urbanczyk]

OK, I'll amend the title myself.

[adam-urbanczyk]

I'm not sure that we are on the same page though - to me last example in the sketch docs shows how to place a sketch in an empty workplane.

[Willy-Schnackenpfefferhausen]

I agree with your title.

"... last example in the sketch docs shows how to place a sketch in an empty workplane." Fair enough, but I did not know what to do with a sketch in an empty workplane other than to loft.