Creating shell from complex shape

[Sean Leavey]

I'm trying to create a shell from a solid heart shape by removing the
face in the Z plane of the attached image (marked with the red X).

Selecting the face with .faces("+Z") or .faces("-Z") then .shell(0.1)
results in the error "Standard_NoSuchObject: NCollection_DataMap::Find":

def heart():
wire = cq.Workplane("XY") \
.lineTo(2, 2) \
.threePointArc((4, 1), (3.5, 0)) \
.mirrorX()

return wire \
.extrude(1.5) \
.edges(">Z") \
.fillet(1.2)

result = heart().faces("+Z").shell(0.1)

I can verify there is a +Z face by typing heart().faces("+Z").size() in
the console and getting 1 in return.

What's wrong with my code? Any advice would be much appreciated.

[Jeremy Wright]

The following simplified code gives me the BRep_API: command not done error that says the CAD kernel had some sort of internal issue when applying the shell.

wire = (cq.Workplane("XY")

         .lineTo(2, 2)
         .threePointArc((4, 1), (3.5, 0))

         .mirrorX())

heart = wire.extrude(1.5)

heart = heart.faces(">Z").shell(0.1)

show_object(heart)

I'm guessing there's a community member who can figure out a work around, but this is an alternative you could explore, although your fillet was too large for your wall thickness so I had to decrease it.

wire = (cq.Workplane("XY")

         .lineTo(2, 2)
         .threePointArc((4, 1), (3.5, 0))

         .mirrorX())

wire2 = wire.offset2D(-0.1).translate((0, 0, 0.1))

heart = wire.extrude(1.5)

heart = heart.wires("<Z").toPending().offset2D(-0.1).cutBlind(1.4).edges(">Z").fillet(0.5)

show_object(heart)

You could also consider making the heart sketch parametric and using that instead of messing with toPending().offset2D().

[Ami Fischman]

Shelling using kind='intersection', and doing it before filleting, and increasing shell wall size to accomodate the fillet, makes it work (cadhub preview):

import cadquery as cq

def heart():

    wire = (cq.Workplane("XY")

        .lineTo(2, 2)

        .threePointArc((4, 1), (3.5, 0))

        .mirrorX()

    )

    return (

        wire

        .extrude(1.5)

        .faces("<Z").shell(0.3, kind='intersection')

        .edges(">Z").fillet(0.1)

    )

show_object(heart())

[Jeremy Wright]

I see some visual artifacts in the render that make me wonder if it's a valid shape though. Do you see those as well? The fillets have some extra edges and some of the features are transparent.

[Ami Fischman]

I also see visual artifacts but the generated STL looks good and PrusaSlicer seems to do the right thing.

Looks like a rendering bug.

[Sean Leavey]

Thanks both for your help! Both solutions give nice looking shapes but I was intentionally abusing the fillet feature to create that rounded effect on the rear.

I modified Ami's code to increase the fillet to 1 and it seems like it will work (haven't checked the STL though) but anything beyond that and I start to see weird artifacts (screenshot attached for a 1.3 fillet).

I like the idea of filleting *after* shelling though, that's not something I'd thought to try.

I also tried a different approach, creating a copy of the heart in the original code I posted, scaling it down, and cutting it out of the original heart. It doesn't produce uniformly thick walls as `shell` would do, but it's good enough for my application (a soap mould):

import cadquery as cq

def scale(workplane, x, y=None, z=None):
    """Scale workplane.
    
    From mbway: https://github.com/CadQuery/cadquery/issues/638
    """
    y = y if y is not None else x
    z = z if z is not None else x
    t = cq.Matrix([
        [x, 0, 0, 0],
        [0, y, 0, 0],
        [0, 0, z, 0],
        [0, 0, 0, 1]
    ])
    
    return workplane.newObject([
        o.transformGeometry(t) if isinstance(o, cq.Shape) else o
        for o in workplane.objects
    ])

def heart(scale=1):

    wire = cq.Workplane("XY") \

        .lineTo(scale*2, scale*2) \
        .threePointArc((scale*4, scale*1), (scale*3.5, 0)) \
        .mirrorX()
    
    return wire \
        .extrude(scale*1.5) \
        .edges(">Z") \
        .fillet(scale*1.2)

result = heart().cut(scale(heart(), 0.9).translate([0.2, 0, 0]))

Screenshots attached of the front and rear (latter showing the effect I'm using the fillet to achieve).

For the record I'm still interested to see if a shell can be made to work for the shape and fillet specified in the original post.

Thanks again for your help so far!

[Roger Maitland]

I love this question 😉 - I think this version produces walls of constant thickness:

import cadquery as cq

outer = (

cq.Workplane("XY")

.lineTo(2, 2)

.threePointArc((4, 1), (3.5, 0))

.mirrorX()

.extrude(-1.5)

.edges("<Z")

.fillet(1.2)

)

inner = (

cq.Workplane("XY")

.lineTo(2, 2)

.threePointArc((4, 1), (3.5, 0))

.mirrorX()

.offset2D(-0.1, kind="intersection")

.extrude(-1.4)

.edges("<Z")

.fillet(1.1)

)

heart = outer - inner

show_object(heart, name="heart")

which generates:

I find the "BRep_API: command not done" message frustrating as it doesn't really give any information about why.  I understand that this is a core issue and not specific to CadQuery but it definitely increases the slope of the learning curve.

Cheers,

Roger

--
cadquery home: https://github.com/CadQuery/cadquery
post issues at https://github.com/CadQuery/cadquery/issues
run it at home at : https://github.com/CadQuery/CQ-editor
---
You received this message because you are subscribed to the Google Groups "CadQuery" group.
To unsubscribe from this group and stop receiving emails from it, send an email to cadquery+u...@googlegroups.com.
To view this discussion on the web visit https://groups.google.com/d/msgid/cadquery/ebd69e9e-720b-4940-b2b2-6bde9c81dd47n%40googlegroups.com.

[Sean Leavey]

Wow, that's perfect! Thanks for that.