Drafting

[tshead]

Thanks for build123d, I really enjoy the programmatic workflow. I am most interested in producing technical drawings for manual machining, and I’ve gotten to a place where I have a nice clean separation between defining the part, and defining the drawing. However, it relies on having a sketch I can add to the drawing, where I’d rather create projections of the 3D part. The project() operation seems like the answer, but I’ve yet to get it to work; is there an example somewhere that I’ve missed? I didn’t see anything in the tutorials.

Thanks in advance,
Tim

# Create the 3D part.
with BuildPart() as part:
    with BuildSketch() as shape:
        with BuildLine():
            l1 = Polyline((20, 40), (-40, 40), (-40, -40), (20, -40))
            RadiusArc(l1 @ 0, l1 @ 1, 50)
        make_face()
        offset(amount=10)
    extrude(amount=10)

part

# Create the drawing with dimensions.
draft = Draft()

with BuildSketch() as drawing:
    add(shape)
    
    # Create a bounding box so we can get overall dimensions.
    box = bounding_box(objects=shape.sketch, mode=Mode.PRIVATE)
    
    ExtensionLine(border=box.edges().sort_by(Axis.X)[0], offset=-10, draft=draft)
    ExtensionLine(border=box.edges().sort_by(Axis.Y)[0], offset=-10, draft=draft)
    TechnicalDrawing(page_size=(PageSize.A3))

drawing

[gumyr]

For this drawing you likely want to create a section of your part and use that in the drawing:

# Create the 3D part.
with BuildPart() as part:
    with BuildSketch() as shape:
        with BuildLine():
            l1 = Polyline((20, 40), (-40, 40), (-40, -40), (20, -40))
            RadiusArc(l1 @ 0, l1 @ 1, 50)
        make_face()
        offset(amount=10)
    extrude(amount=10)
    drawing_slice = section(section_by=Plane.XY)

# Create the drawing with dimensions.
draft = Draft()

with BuildSketch() as drawing:
    add(drawing_slice)

    # Create a bounding box so we can get overall dimensions.
    box = bounding_box(objects=drawing_slice, mode=Mode.PRIVATE)

    ExtensionLine(border=box.edges().sort_by(Axis.X)[0], offset=-10, draft=draft)
    ExtensionLine(border=box.edges().sort_by(Axis.Y)[0], offset=-10, draft=draft)
    TechnicalDrawing(page_size=(PageSize.A3))

If you'd like to include a "3D" view into your drawing you can use:

visible, hidden = part.part.project_to_viewport((-50, -20, 50))

and add that (with or without hidden lines).

There should be a whole section in the docs on how to create technical drawings. In addition, I can imagine much more sophisticated features that would help with placement of ExtensionLines to achieve a better overall document.

[tshead]

@gumyr Thanks a lot for the feedback, that gets me much further along … one more question, I notice that the visible and hidden results from project_to_viewport are instances of ShapeList … although I can view them with jupyter_cadquery just fine, it seems that ShapeList can’t be added to a sketch - is there a trick to that? As a minimal example continuing from the above:

visible, hidden = part.part.project_to_viewport((-50, 20, 50))

with BuildSketch() as drawing:
    add(visible)

drawing

---------------------------------------------------------------------------
ValueError                                Traceback (most recent call last)
File ~/miniconda3/envs/default/lib/python3.12/site-packages/IPython/core/formatters.py:925, in IPythonDisplayFormatter.__call__(self, obj)
    923 method = get_real_method(obj, self.print_method)
    924 if method is not None:
--> 925     method()
    926     return True

File ~/miniconda3/envs/default/lib/python3.12/site-packages/jupyter_cadquery/tools.py:41, in auto_show.<locals>.<lambda>(cad_obj)
     39 if HAS_BUILD123D:
     40     bd.BuildPart._ipython_display_ = lambda cad_obj: show(cad_obj)
---> 41     bd.BuildSketch._ipython_display_ = lambda cad_obj: show(cad_obj)
     42     bd.BuildLine._ipython_display_ = lambda cad_obj: show(cad_obj)
     43     bd.ShapeList._ipython_display_ = lambda cad_obj: show(cad_obj)

File ~/miniconda3/envs/default/lib/python3.12/site-packages/jupyter_cadquery/cad_objects.py:1005, in show(names, colors, alphas, *cad_objs, **kwargs)
   1001     kwargs["grid"] = (kwargs["grid"], False, False)
   1003 if cad_objs:
-> 1005     assembly = to_assembly(
   1006         *cad_objs,
   1007         names=names,
   1008         colors=colors,
   1009         alphas=alphas,
   1010         render_mates=render_mates,
   1011         mate_scale=mate_scale,
   1012         default_color=default_color,
   1013         show_parent=show_parent,
   1014     )
   1016     if assembly is None:
   1017         raise ValueError("%s cannot be viewed" % cad_objs)

File ~/miniconda3/envs/default/lib/python3.12/site-packages/jupyter_cadquery/cad_objects.py:638, in to_assembly(names, colors, alphas, name, render_mates, mate_scale, default_color, show_parent, *cad_objs)
    636 if hasattr(cad_obj, "_obj_name"):  # BuildPart, BuildSketch, BuildLine
    637     _debug(f"CAD Obj {obj_id}: {type(cad_obj)}")
--> 638     cad_obj = getattr(cad_obj, cad_obj._obj_name)
    639     if not isinstance(cad_obj, bd.Compound):
    640         cad_obj = Shape.cast(cad_obj.wrapped)

File ~/miniconda3/envs/default/lib/python3.12/site-packages/build123d/build_sketch.py:85, in BuildSketch.sketch(self)
     83 global_objs = []
     84 for plane in workplanes:
---> 85     global_objs.append(plane.from_local_coords(self._obj))
     86 return Sketch(Compound(global_objs).wrapped)

File ~/miniconda3/envs/default/lib/python3.12/site-packages/build123d/geometry.py:2433, in Plane.from_local_coords(self, obj)
   2422 def from_local_coords(self, obj: Union[tuple, Vector, Any, BoundBox]):
   2423     """Reposition the object relative from this plane
   2424 
   2425     Args:
   (...)
   2431 
   2432     """
-> 2433     return self._to_from_local_coords(obj, False)

File ~/miniconda3/envs/default/lib/python3.12/site-packages/build123d/geometry.py:2404, in Plane._to_from_local_coords(self, obj, to_from)
   2402     return_value = obj.transform_shape(transform_matrix)
   2403 else:
-> 2404     raise ValueError(
   2405         f"Unable to repositioned type {type(obj)} with respect to local coordinates"
   2406     )
   2407 return return_value

ValueError: Unable to repositioned type <class 'NoneType'> with respect to local coordinates

Many thanks,
Tim

[gumyr]

The results of project_to_viewport are two ShapeLists of Edges which have zero width so they can't be directly added to the Sketch as Sketches are collections of Faces. To make them visible one needs to add width to these Edges which can be done with the trace operation:

visible, hidden = part.part.project_to_viewport((-50, -20, 50))

with BuildSketch() as drawing:
    trace(visible, 1)
    TechnicalDrawing(page_size=(PageSize.A3))

Here I've set the line width to 1.

Another option that is probably more flexible is to create new Sketch object of the tracing so it can be positioned and added easily:

visible, hidden = part.part.project_to_viewport((-50, -20, 50))
visible_lines = scale(trace(visible, 1), by=0.75)
visible_lines.position += (-120, 75)

# Create the drawing with dimensions.
draft = Draft()

with BuildSketch() as drawing:
    add(visible_lines)
    # trace(visible, 1)

    add(drawing_slice)

    # Create a bounding box so we can get overall dimensions.
    box = bounding_box(objects=drawing_slice, mode=Mode.PRIVATE)

    ExtensionLine(border=box.edges().sort_by(Axis.X)[0], offset=-10, draft=draft)
    ExtensionLine(border=box.edges().sort_by(Axis.Y)[0], offset=-10, draft=draft)
    TechnicalDrawing(page_size=(PageSize.A3))

All of this needs to go into the missing "How to create Technical Drawings" documentation page.

[tshead]

@gumyr Thanks for the response, particularly the clarification that a Sketch is a collection of faces - that was not obvious to me. Maybe I’ll submit a writeup if I can get this toy example fully dimensioned.

Thanks again,
Tim