There are two primary APIs provided by build123d: builder and algebra. The builder api may be easier for new users as it provides some assistance and shortcuts; however, if you know what a Quaternion is you might prefer the algebra API which allows CAD objects to be created in the style of mathematical equations. Both API can be mixed in the same model with the exception that the algebra API can't be used from within a builder context. As with music, there is no "best" genre or API, use the one you prefer or both if you like.
The following key concepts will help new users understand build123d quickly.
Topology, in the context of 3D modeling and computational geometry, is the branch of mathematics that deals with the properties and relationships of geometric objects that are preserved under continuous deformations. In the context of CAD and modeling software like build123d, topology refers to the hierarchical structure of geometric elements (vertices, edges, faces, etc.) and their relationships in a 3D model. This structure defines how the components of a model are connected, enabling operations like Boolean operations, transformations, and analysis of complex shapes. Topology provides a formal framework for understanding and manipulating geometric data in a consistent and reliable manner.
The following are the topological objects that compose build123d objects:
~topology.Vertex
A Vertex is a data structure representing a 0D topological element. It defines a precise point in 3D space, often at the endpoints or intersections of edges in a 3D model. These vertices are part of the topological structure used to represent complex shapes in build123d.
~topology.Edge
An Edge in build123d is a fundamental geometric entity representing a 1D element in a 3D model. It defines the shape and position of a 1D curve within the model. Edges play a crucial role in defining the boundaries of faces and in constructing complex 3D shapes.
~topology.Wire
A Wire in build123d is a topological construct that represents a connected sequence of Edges, forming a 1D closed or open loop within a 3D model. Wires define the boundaries of faces and can be used to create complex shapes, making them essential for modeling in build123d.
~topology.Face
A Face in build123d represents a 2D surface in a 3D model. It defines the boundary of a region and can have associated geometric and topological data. Faces are vital for shaping solids, providing surfaces where other elements like edges and wires are connected to form complex structures.
~topology.Shell
A Shell in build123d represents a collection of Faces, defining a closed, connected volume in 3D space. It acts as a container for organizing and grouping faces into a single shell, essential for defining complex 3D shapes like solids or assemblies within the build123d modeling framework.
~topology.Solid
A Solid in build123d is a 3D geometric entity that represents a bounded volume with well-defined interior and exterior surfaces. It encapsulates a closed and watertight shape, making it suitable for modeling solid objects and enabling various Boolean operations such as union, intersection, and subtraction.
~topology.Compound
A Compound in build123d is a container for grouping multiple geometric shapes. It can hold various types of entities, such as vertices, edges, wires, faces, shells, or solids, into a single structure. This makes it a versatile tool for managing and organizing complex assemblies or collections of shapes within a single container.
~topology.Shape
A Shape in build123d represents a fundamental building block in 3D modeling. It encompasses various topological elements like vertices, edges, wires, faces, shells, solids, and compounds. The Shape class is the base class for all of the above topological classes.
One can use the ~topology.Shape.show_topology
method to display the topology of a shape as shown here for a unit cube:
Solid at 0x7f94c55430f0, Center(0.5, 0.5, 0.5)
└── Shell at 0x7f94b95835f0, Center(0.5, 0.5, 0.5)
├── Face at 0x7f94b95836b0, Center(0.0, 0.5, 0.5)
│ └── Wire at 0x7f94b9583730, Center(0.0, 0.5, 0.5)
│ ├── Edge at 0x7f94b95838b0, Center(0.0, 0.0, 0.5)
│ │ ├── Vertex at 0x7f94b9583470, Center(0.0, 0.0, 1.0)
│ │ └── Vertex at 0x7f94b9583bb0, Center(0.0, 0.0, 0.0)
│ ├── Edge at 0x7f94b9583a30, Center(0.0, 0.5, 1.0)
│ │ ├── Vertex at 0x7f94b9583030, Center(0.0, 1.0, 1.0)
│ │ └── Vertex at 0x7f94b9583e70, Center(0.0, 0.0, 1.0)
│ ├── Edge at 0x7f94b9583770, Center(0.0, 1.0, 0.5)
│ │ ├── Vertex at 0x7f94b9583bb0, Center(0.0, 1.0, 1.0)
│ │ └── Vertex at 0x7f94b9583e70, Center(0.0, 1.0, 0.0)
│ └── Edge at 0x7f94b9583db0, Center(0.0, 0.5, 0.0)
│ ├── Vertex at 0x7f94b9583e70, Center(0.0, 1.0, 0.0)
│ └── Vertex at 0x7f94b95862f0, Center(0.0, 0.0, 0.0)
...
└── Face at 0x7f94b958d3b0, Center(0.5, 0.5, 1.0)
└── Wire at 0x7f94b958d670, Center(0.5, 0.5, 1.0)
├── Edge at 0x7f94b958e130, Center(0.0, 0.5, 1.0)
│ ├── Vertex at 0x7f94b958e330, Center(0.0, 1.0, 1.0)
│ └── Vertex at 0x7f94b958e770, Center(0.0, 0.0, 1.0)
├── Edge at 0x7f94b958e630, Center(0.5, 1.0, 1.0)
│ ├── Vertex at 0x7f94b958e8b0, Center(1.0, 1.0, 1.0)
│ └── Vertex at 0x7f94b958ea70, Center(0.0, 1.0, 1.0)
├── Edge at 0x7f94b958e7b0, Center(1.0, 0.5, 1.0)
│ ├── Vertex at 0x7f94b958ebb0, Center(1.0, 1.0, 1.0)
│ └── Vertex at 0x7f94b958ed70, Center(1.0, 0.0, 1.0)
└── Edge at 0x7f94b958eab0, Center(0.5, 0.0, 1.0)
├── Vertex at 0x7f94b958eeb0, Center(1.0, 0.0, 1.0)
└── Vertex at 0x7f94b9592170, Center(0.0, 0.0, 1.0)
Users of build123d will often reference topological objects as part of the process of creating the object as described below.
The three builders, BuildLine
, BuildSketch
, and BuildPart
are tools to create new objects - not the objects themselves. Each of the objects and operations applicable to these builders create objects of the standard CadQuery Direct API, most commonly Compound
objects. This is opposed to CadQuery's Fluent API which creates objects of the Workplane
class which frequently needed to be converted back to base class for further processing.
One can access the objects created by these builders by referencing the appropriate instance variable. For example:
with BuildPart() as my_part:
...
show_object(my_part.part)
with BuildSketch() as my_sketch:
...
show_object(my_sketch.sketch)
with BuildLine() as my_line:
...
show_object(my_line.line)
One might expect to have to reference a builder's instance variable when using objects or operations that impact that builder like this:
with BuildPart() as part_builder:
Box(part_builder, 10,10,10)
Instead, build123d determines from the scope of the object or operation which builder it applies to thus eliminating the need for the user to provide this information - as follows:
with BuildPart() as part_builder:
Box(10,10,10)
with BuildSketch() as sketch_builder:
Circle(2)
In this example, Box
is in the scope of part_builder
while Circle
is in the scope of sketch_builder
.
As build123d is a 3D CAD package one must be able to position objects anywhere. As one frequently will work in the same plane for a sequence of operations, the first parameter(s) of the builders is a (sequence of) workplane(s) which is (are) used to aid in the location of features. The default workplane in most cases is the Plane.XY
where a tuple of numbers represent positions on the x and y axes. However workplanes can be generated on any plane which allows users to put a workplane where they are working and then work in local 2D coordinate space.
with BuildPart(Plane.XY) as example:
... # a 3D-part
with BuildSketch(example.faces().sort_by(sort_by=Axis.Z)[0]) as bottom:
...
with BuildSketch(Plane.XZ) as vertical:
...
with BuildSketch(example.faces().sort_by(sort_by=Axis.Z)[-1]) as top:
...
When BuildPart
is invoked it creates the workplane provided as a parameter (which has a default of the Plane.XY
). The bottom
sketch is therefore created on the Plane.XY
but with the normal reversed to point down. Subsequently the user has created the vertical
(Plane.XZ
`) sketch. All objects or operations within the scope of a workplane will automatically be orientated with respect to this plane so the user only has to work with local coordinates.
As shown above, workplanes can be created from faces as well. The top
sketch is positioned on top of example
by selecting its faces and finding the one with the greatest z value.
One is not limited to a single workplane at a time. In the following example all six faces of the first box is used to define workplanes which are then used to position rotated boxes.
import build123d as bd
with bd.BuildPart() as bp:
bd.Box(3, 3, 3)
with bd.BuildSketch(*bp.faces()):
bd.Rectangle(1, 2, rotation=45)
bd.extrude(amount=0.1)
This is the result:
A ~geometry.Location
represents a combination of translation and rotation applied to a topological or geometric object. It encapsulates information about the spatial orientation and position of a shape within its reference coordinate system. This allows for efficient manipulation of shapes within complex assemblies or transformations. The location is typically used to position shapes accurately within a 3D scene, enabling operations like assembly, and boolean operations. It's an essential component in build123d for managing the spatial relationships of geometric entities, providing a foundation for precise 3D modeling and engineering applications.
The topological classes (sub-classes of ~topology.Shape
) and the geometric classes ~geometry.Axis
and ~geometry.Plane
all have a location
property. The ~geometry.Location
class itself has position
and orientation
properties that have setters and getters as shown below:
>>> from build123d import * >>> # Create an object and extract its location >>> b = Box(1, 1, 1) >>> box_location = b.location >>> box_location (p=(0.00, 0.00, 0.00), o=(-0.00, 0.00, -0.00)) >>> # Set position and orientation independently >>> box_location.position = (1, 2, 3) >>> box_location.orientation = (30, 40, 50) >>> box_location.position Vector: (1.0, 2.0, 3.0) >>> box_location.orientation Vector: (29.999999999999993, 40.00000000000002, 50.000000000000036)
Combining the getter and setter enables relative changes as follows:
>>> # Relative change >>> box_location.position += (3, 2, 1) >>> box_location.position Vector: (4.0, 4.0, 4.0)
There are also four methods that are used to change the location of objects:
~topology.Shape.locate
- absolute change of this object~topology.Shape.located
- absolute change of copy of this object~topology.Shape.move
- relative change of this object~topology.Shape.moved
- relative change of copy of this object
Locations can be combined with the *
operator and have their direction flipped with the -
operator.
When positioning objects or operations within a builder Location Contexts are used. These function in a very similar was to the builders in that they create a context where one or more locations are active within a scope. For example:
with BuildPart():
with Locations((0,10),(0,-10)):
Box(1,1,1)
with GridLocations(x_spacing=5, y_spacing=5, x_count=2, y_count=2):
Sphere(1)
Cylinder(1,1)
In this example Locations
creates two positions on the current workplane at (0,10) and (0,-10). Since Box
is within the scope of Locations
, two boxes are created at these locations. The GridLocations
context creates four positions which apply to the Sphere
. The Cylinder
is out of the scope of GridLocations
but in the scope of Locations
so two cylinders are created.
Note that these contexts are creating Location objects not just simple points. The difference isn't obvious until the PolarLocations
context is used which can also rotate objects within its scope - much as the hour and minute indicator on an analogue clock.
Also note that the locations are local to the current location(s) - i.e. Locations
can be nested. It's easy for a user to retrieve the global locations:
with Locations(Plane.XY, Plane.XZ):
locs = GridLocations(1, 1, 2, 2)
for l in locs:
print(l)
Location(p=(-0.50,-0.50,0.00), o=(0.00,-0.00,0.00))
Location(p=(-0.50,0.50,0.00), o=(0.00,-0.00,0.00))
Location(p=(0.50,-0.50,0.00), o=(0.00,-0.00,0.00))
Location(p=(0.50,0.50,0.00), o=(0.00,-0.00,0.00))
Location(p=(-0.50,-0.00,-0.50), o=(90.00,-0.00,0.00))
Location(p=(-0.50,0.00,0.50), o=(90.00,-0.00,0.00))
Location(p=(0.50,0.00,-0.50), o=(90.00,-0.00,0.00))
Location(p=(0.50,0.00,0.50), o=(90.00,-0.00,0.00))
When one is operating on an existing object, e.g. adding a fillet to a part, an iterable of objects is often required (often a ShapeList).
Here is the definition of ~operations_generic.fillet
to help illustrate:
def fillet(
objects: Union[Union[Edge, Vertex], Iterable[Union[Edge, Vertex]]],
radius: float,
):
To use this fillet operation, an edge or vertex or iterable of edges or vertices must be provided followed by a fillet radius with or without the keyword as follows:
with BuildPart() as pipes:
Box(10, 10, 10, rotation=(10, 20, 30))
...
fillet(pipes.edges(Select.LAST), radius=0.2)
Here the fillet accepts the iterable ShapeList of edges from the last operation of the pipes
builder and a radius is provided as a keyword argument.
Almost all objects or operations have a mode
parameter which is defined by the Mode
Enum class as follows:
class Mode(Enum):
ADD = auto()
SUBTRACT = auto()
INTERSECT = auto()
REPLACE = auto()
PRIVATE = auto()
The mode
parameter describes how the user would like the object or operation to interact with the object within the builder. For example, Mode.ADD
will integrate a new object(s) in with an existing part
. Note that a part doesn't necessarily have to be a single object so multiple distinct objects could be added resulting is multiple objects stored as a Compound
object. As one might expect Mode.SUBTRACT
, Mode.INTERSECT
, and Mode.REPLACE
subtract, intersect, or replace (from) the builder's object. Mode.PRIVATE
instructs the builder that this object should not be combined with the builder's object in any way.
Most commonly, the default mode
is Mode.ADD
but this isn't always true. For example, the Hole
classes use a default Mode.SUBTRACT
as they remove a volume from the part under normal circumstances. However, the mode
used in the Hole
classes can be specified as Mode.ADD
or Mode.INTERSECT
to help in inspection or debugging.
build123d stores points (to be specific Location
(s)) internally to be used as positions for the placement of new objects. By default, a single location will be created at the origin of the given workplane such that:
with BuildPart() as pipes:
Box(10, 10, 10, rotation=(10, 20, 30))
will create a single 10x10x10 box centered at (0,0,0) - by default objects are centered. One can create multiple objects by pushing points prior to creating objects as follows:
with BuildPart() as pipes:
with Locations((-10, -10, -10), (10, 10, 10)):
Box(10, 10, 10, rotation=(10, 20, 30))
which will create two boxes.
To orient a part, a rotation
parameter is available on BuildSketch
and BuildPart APIs. When working in a sketch, the rotation is a single angle in degrees so the parameter is a float. When working on a part, the rotation is a three dimensional Rotation object of the form Rotation(<about x>, <about y>, <about z>) although a simple three tuple of floats can be used as input. As 3D rotations are not cumulative, one can combine rotations with the ` operator like this: ``Rotation(10, 20, 30) Rotation(0, 90, 0)to generate any desired rotation. .. hint:: Experts Only
Locationswill accept
Locationobjects for input which allows one to specify both the position and orientation. However, the orientation is often determined by the
Planethat an object was created on.
Rotationis a subclass of
Locationand therefore will also accept a position component. Builder's Pending Objects ========================= When a builder exits, it will push the object created back to its parent if there was one. Here is an example: .. code-block:: python height, width, thickness, f_rad = 60, 80, 20, 10 with BuildPart() as pillow_block: with BuildSketch() as plan: Rectangle(width, height) fillet(plan.vertices(), radius=f_rad) extrude(amount=thickness)
BuildSketchexits after the
filletoperation and when doing so it transfers the sketch to the
pillow_blockinstance of
BuildPartas the internal instance variable
pending_faces. This allows the
extrudeoperation to be immediately invoked as it extrudes these pending faces into
Solidobjects. Likewise,
loftwould take all of the
pending_facesand attempt to create a single
Solidobject from them. Normally the user will not need to interact directly with pending objects; however, one can see pending Edges and Faces with
<builder_instance>.pending_edgesand
<builder_instance>.pending_facesattributes. In the above example, by adding a
print(pillow_block.pending_faces)prior to the
extrude(amount=thickness)the pending
Facefrom the
BuildSketch`` will be displayed.