Weird "Fillets requires that edges be selected" exception

[KizzyCode]

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To Reproduce

I'm trying to build some gridfinity stuff, therefore I'm trying to to build the baseplate in CadQuery. However I'm getting some weird Fillets requires that edges be selected-exception.

(The following code are cells from a Jupyter-notebook, where each ##### marks a different cell)

rounding_diameter = 7_500
outer_width = 42_000

layer0_inner = 42_000 - ((2_150 + 700) * 2)
layer0_height = 700
layer0_rounding_diameter_inner = rounding_diameter - (outer_width - layer0_inner)

layer1_inner = 42_000 - (2_150 * 2)
layer1_height = 1_800
layer1_rounding_diameter_inner = rounding_diameter - (outer_width - layer1_inner)

layer2_inner = 42_000 - (2_150 * 2)
layer2_height = 1_900
layer2_rounding_diameter_inner = rounding_diameter - (outer_width - layer2_inner)

#####

from cadquery import Workplane

object = Workplane()\
    .box(outer_width, outer_width, layer0_height, centered=[True, True, False])\
    .faces(">Z")\
        .workplane(invert=True)\
        .box(layer0_inner, layer0_inner, layer0_height, centered=[True, True, False], combine="cut")\
    .edges("|Z and (>X or <X)")\
        .fillet(rounding_diameter / 2)\
    .edges("|Z")\
        .fillet(layer0_rounding_diameter_inner / 2)

display(object)

#####

object = object\
    .faces(">Z")\
        .workplane()\
        .box(outer_width, outer_width, layer1_height, centered=[True, True, False])\
    .faces(">Z")\
        .workplane(invert=True)\
        .box(layer1_inner, layer1_inner, layer1_height, centered=[True, True, False], combine="cut")\
    .edges("|Z and (>X or <X)")\
        .fillet(rounding_diameter / 2)\
    .edges("|Z")\
        .fillet(layer1_rounding_diameter_inner / 2)

display(object)

#####

object = object\
    .faces(">Z")\
        .workplane()\
        .box(outer_width, outer_width, layer2_height, centered=[True, True, False])\
    .faces(">Z")\
        .workplane(invert=True)\
        .box(layer2_inner, layer2_inner, layer2_height, centered=[True, True, False], combine="cut")\
    .edges("|Z and (>X or <X)")\
        .fillet(rounding_diameter / 2)\ # <--- THIS IS THE LINE TRIGGERING THE EXCEPTION
    .edges("|Z")\
        .fillet(layer2_rounding_diameter_inner / 2)

display(object)

The weird thing is: If I change the rounding_diameter / 2 to either rounding_diameter / 2.00001 OR rounding_diameter / 1.99999, it does not throw... for me this looks like some kind of floating point error; but then I'm a noob regarding CAD-kernels, and I'm pretty confused that it works with a deviation in both directions. Also I'm a newby with CadQuery, so please bear with me if I'm completely misunderstanding some concepts here 🙈

Backtrace

{
	"name": "StdFail_NotDone",
	"message": "BRep_API: command not done",
	"stack": "---------------------------------------------------------------------------
StdFail_NotDone                           Traceback (most recent call last)
Cell In[117], line 9
      1 object = object\\
      2     .faces(\">Z\")\\
      3         .workplane()\\
      4         .box(outer_width, outer_width, layer2_height, centered=[True, True, False])\\
      5     .faces(\">Z\")\\
      6         .workplane(invert=True)\\
      7         .box(layer2_inner, layer2_inner, layer2_height, centered=[True, True, False], combine=\"cut\")\\
      8     .edges(\"|Z and (>X or <X)\")\\
----> 9         .fillet(rounding_diameter / 2)\\
     10     .edges(\"|Z\")\\
     11         .fillet(layer2_rounding_diameter_inner / 2)
     13 display(object)

File /usr/local/lib/python3.11/dist-packages/cadquery/cq.py:1304, in Workplane.fillet(self, radius)
   1301 if len(edgeList) < 1:
   1302     raise ValueError(\"Fillets requires that edges be selected\")
-> 1304 s = solid.fillet(radius, edgeList)
   1305 return self.newObject([s.clean()])

File /usr/local/lib/python3.11/dist-packages/cadquery/occ_impl/shapes.py:2780, in Mixin3D.fillet(self, radius, edgeList)
   2777 for e in nativeEdges:
   2778     fillet_builder.Add(radius, e)
-> 2780 return self.__class__(fillet_builder.Shape())

StdFail_NotDone: BRep_API: command not done"
}

Environment

OS: VSCode dev container running Debian on M1Pro-MacBook Pro:

FROM mcr.microsoft.com/devcontainers/base:debian

ENV APT_PACKAGES libgl1 libnlopt0 libnlopt-cxx0 python3 python3-dev python3-nlopt python3-pip
ENV DEBIAN_FRONTEND noninteractive
RUN apt-get update \
    && apt-get upgrade --yes \
    && apt-get install --yes --no-install-recommends ${APT_PACKAGES} \
    && apt-get autoremove --yes \
    && apt-get clean

RUN pip install --break-system-packages \
    ipykernel
# Manually install top-level dependencies of `cadquery` except `nlopt`
RUN pip install --break-system-packages \
    casadi \
    ezdxf \
    multimethod==1.9.1 \
    nptyping==2.0.1 \
    path \
    typish \
    https://github.com/CadQuery/ocp-build-system/releases/download/7.7.2.0/cadquery_ocp-7.7.2-cp311-cp311-manylinux_2_35_aarch64.whl
# Install `cadquery` without automatic dependency resolution
RUN pip install --break-system-packages --no-deps \
    cadquery

Also see my attached workspace if it is any use: Gridfinity.zip

[lorenzncode]

It looks like you are creating rounded walls. In general, it's recommended to create this kind of shape in 2D. I don't know the root cause of the issue with your code, however, I'd suggest to try moving the fillet to 2D with something like this:

import cadquery as cq


def make_wall(w1, w2, d1, d2) -> cq.Sketch:
    return (
        cq.Sketch()
        .rect(w1, w1, tag="outer")
        .rect(w2, w2, mode="s", tag="inner")
        .vertices(tag="outer")
        .fillet(d1 / 2)
        .vertices(tag="inner")
        .fillet(d2 / 2)
    )


res = (
    cq.Workplane()
    .placeSketch(make_wall(50, 40, 10, 5))
    .extrude(10)
    .faces(">Z")
    .workplane()
    .placeSketch(make_wall(50, 45, 10, 5))
    .extrude(5)
)

[KizzyCode]

Thanks, will try it like this instead. Please feel free to close this if it is out-of-scope or probably a problem with the underlying CAD-kernel 😊

[lorenzncode]

Yes AFAICT it's a kernel issue. Here is a minimal example. It fails with same error as original code.:

import cadquery as cq

b0 = cq.Workplane().box(100, 100, 5).edges(">XY").fillet(10)

b1 = (
    b0.faces(">Z")
    .box(100, 100, 5, centered=[True, True, False])
    .edges(">XY")
    .fillet(10)
)

A workaround could be to set combine to False in b1, then union after the b1 fillet

b1 = (
    b0.faces(">Z")
    .box(100, 100, 5, centered=[True, True, False], combine=False)
    .edges(">XY")
    .fillet(10)
)

b1 = b1.union(b0)

... or move the fillet to 2D as in the previous example.