Concepts

3D BREP Topology Concepts

Before talking about CadQuery, it makes sense to talk a little about 3D CAD topology. CadQuery is based upon the OpenCascade kernel, which uses Boundary Representations (BREP) for objects. This just means that objects are defined by their enclosing surfaces.

When working in a BREP system, these fundamental constructs exist to define a shape (working up the food chain):

vertex

a single point in space

edge

a connection between two or more vertices along a particular path (called a curve)

wire

a collection of edges that are connected together.

face

a set of edges or wires that enclose a surface

shell

a collection of faces that are connected together along some of their edges

solid

a shell that has a closed interior

compound

a collection of solids

When using CadQuery, all of these objects are created, hopefully with the least possible work. In the actual CAD kernel, there is another set of Geometrical constructs involved as well. For example, an arc-shaped edge will hold a reference to an underlying curve that is a full circle, and each linear edge holds underneath it the equation for a line. CadQuery shields you from these constructs.

Workplane class

The Workplane class contains the currently selected objects (a list of Shapes, Vectors or Locations in the objects attribute), the modelling context (in the ctx attribute), and CadQuery’s fluent api methods. It is the main class that users will instantiate.

See API Reference to learn more.

Workplanes

Most CAD programs use the concept of Workplanes. If you have experience with other CAD programs you will probably feel comfortable with CadQuery’s Workplanes, but if you don’t have experience then they are an essential concept to understand.

Workplanes represent a plane in space, from which other features can be located. They have a center point and a local coordinate system. Most methods that create an object do so relative to the current workplane.

Usually the first workplane created is the “XY” plane, also known as the “front” plane. Once a solid is defined the most common way to create a workplane is to select a face on the solid that you intend to modify and create a new workplane relative to it. You can also create new workplanes in anywhere in world coordinate system, or relative to other planes using offsets or rotations.

The most powerful feature of workplanes is that they allow you to work in 2D space in the coordinate system of the workplane, and then CadQuery will transform these points from the workplane coordinate system to the world coordinate system so your 3D features are located where you intended. This makes scripts much easier to create and maintain.

See cadquery.Workplane to learn more.

2D Construction

Once you create a workplane, you can work in 2D, and then later use the features you create to make 3D objects. You’ll find all of the 2D constructs you expect – circles, lines, arcs, mirroring, points, etc.

See 2D Operations to learn more.

3D Construction

You can construct 3D primitives such as boxes, wedges, cylinders and spheres directly. You can also sweep, extrude, and loft 2D geometry to form 3D features. Of course the basic primitive operations are also available.

See 3D Operations to learn more.

Selectors

Selectors allow you to select one or more features, in order to define new features. As an example, you might extrude a box, and then select the top face as the location for a new feature. Or, you might extrude a box, and then select all of the vertical edges so that you can apply a fillet to them.

You can select Vertices, Edges, Faces, Solids, and Wires using selectors.

Think of selectors as the equivalent of your hand and mouse, if you were to build an object using a conventional CAD system.

See Selectors to learn more.

Construction Geometry

Construction geometry are features that are not part of the object, but are only defined to aid in building the object. A common example might be to define a rectangle, and then use the corners to define the location of a set of holes.

Most CadQuery construction methods provide a forConstruction keyword, which creates a feature that will only be used to locate other features.

The Stack

As you work in CadQuery, each operation returns a new Workplane object with the result of that operations. Each Workplane object has a list of objects, and a reference to its parent.

You can always go backwards to older operations by removing the current object from the stack. For example:

Workplane(someObject).faces(">Z").first().vertices()

returns a CadQuery object that contains all of the vertices on the highest face of someObject. But you can always move backwards in the stack to get the face as well:

Workplane(someObject).faces(">Z").first().vertices().end()

You can browse stack access methods here: Stack and Selector Methods.

Chaining

All Workplane methods return another Workplane object, so that you can chain the methods together fluently. Use the core Workplane methods to get at the objects that were created.

Each time a new Workplane object is produced during these chained calls, it has a parent attribute that points to the Workplane object that created it. Several CadQuery methods search this parent chain, for example when searching for the context solid. You can also give a Workplane object a tag, and further down your chain of calls you can refer back to this particular object using its tag.

The Context Solid

Most of the time, you are building a single object, and adding features to that single object. CadQuery watches your operations, and defines the first solid object created as the ‘context solid’. After that, any features you create are automatically combined (unless you specify otherwise) with that solid. This happens even if the solid was created a long way up in the stack. For example:

Workplane("XY").box(1, 2, 3).faces(">Z").circle(0.25).extrude(1)

Will create a 1x2x3 box, with a cylindrical boss extending from the top face. It was not necessary to manually combine the cylinder created by extruding the circle with the box, because the default behavior for extrude is to combine the result with the context solid. The hole() method works similarly – CadQuery presumes that you want to subtract the hole from the context solid.

If you want to avoid this, you can specify combine=False, and CadQuery will create the solid separately.

Iteration

CAD models often have repeated geometry, and its really annoying to resort to for loops to construct features. Many CadQuery methods operate automatically on each element on the stack, so that you don’t have to write loops. For example, this:

Workplane("XY").box(1, 2, 3).faces(">Z").vertices().circle(0.5)

Will actually create 4 circles, because vertices() selects 4 vertices of a rectangular face, and the circle() method iterates on each member of the stack.

This is really useful to remember when you author your own plugins. cadquery.Workplane.each() is useful for this purpose.

CadQuery API layers

Once you start to dive a bit more into CadQuery, you may find yourself a bit confused juggling between different types of objects the CadQuery APIs can return. This chapter aims to give an explanation on this topic and to provide background on the underlying implementation and kernel layers so you can leverage more of CadQuery functionality.

CadQuery is composed of 3 different API, which are implemented on top of each other.

1. The Fluent API

2. The Direct API

3. The OCCT API

The Fluent API

What we call the fluent API is what you work with when you first start using CadQuery, the Workplane class and all its methods defines the Fluent API. This is the API you will use and see most of the time, it’s fairly easy to use and it simplifies a lot of things for you. A classic example could be :

part = Workplane("XY").box(1, 2, 3).faces(">Z").vertices().circle(0.5).cutThruAll()

Here we create a Workplane object on which we subsequently call several methods to create our part. A general way of thinking about the Fluent API is to consider the Workplane as your part object and all it’s methods as operations that will affect your part. Often you will start with an empty Workplane, then add more features by calling Workplane methods.

This hierarchical structure of operations modifying a part is well seen with the traditional code style used in CadQuery code. Code written with the CadQuery fluent API will often look like this :

part = Workplane("XY").box(1, 2, 3).faces(">Z").vertices().circle(0.5).cutThruAll()

Or like this :

part = Workplane("XY")
part = part.box(1, 2, 3)
part = part.faces(">Z")
part = part.vertices()
part = part.circle(0.5)
part = part.cutThruAll()

Note

While the first code style is what people default to, it’s important to note that when you write your code like this it’s equivalent as writting it on a single line. It’s then more difficult to debug as you cannot visualize each operation step by step, which is a functionality that is provided by the CQ-Editor debugger for example.

The Direct API

While the fluent API exposes much functionality, you may find scenarios that require extra flexibility or require working with lower level objects.

The direct API is the API that is called by the fluent API under the hood. The 9 topological classes and their methods compose the direct API. These classes actually wrap the equivalent Open CASCADE Technology (OCCT) classes. The 9 topological classes are :

1. Shape

2. Compound

3. CompSolid

4. Solid

5. Shell

6. Face

7. Wire

8. Edge

9. Vertex

Each class has its own methods to create and/or edit shapes of their respective type. As already explained in Concepts there is also some kind of hierarchy in the topological classes. A Wire is made of several edges which are themselves made of several vertices. This means you can create geometry from the bottom up and have a lot of control over it.

For example we can create a circular face like so

circle_wire = Wire.makeCircle(10, Vector(0, 0, 0), Vector(0, 0, 1))
circular_face = Face.makeFromWires(circle_wire, [])

Note

In CadQuery (and OCCT) all the topological classes are shapes, the Shape class is the most abstract topological class. The topological class inherits Mixin3D or Mixin1D which provide aditional methods that are shared between the classes that inherits them.

The direct API as its name suggests doesn’t provide a parent/children data structure, instead each method call directly returns an object of the specified topological type. It is more verbose than the fluent API and more tedious to work with, but as it offers more flexibility (you can work with faces, which is something you can’t do in the fluent API) it is sometimes more convenient than the fluent API.

The OCCT API

Finally we are discussing about the OCCT API. The OCCT API is the lowest level of CadQuery. The direct API is built upon the OCCT API, where the OCCT API in CadQuery is available through OCP. OCP are the Python bindings of the OCCT C++ libraries CadQuery uses. This means you have access to (almost) all the OCCT C++ libraries in Python and in CadQuery. Working with the OCCT API will give you the maximum flexibility and control over you designs, it is however very verbose and difficult to use. You will need to have a strong knowledge of the different C++ libraries to be able to achieve what you want. To obtain this knowledge the most obvious ways are :

1. Read the direct API source code, since it is build upon the OCCT API it is full of example usage.

2. Go through the C++ documentation

Note

The general way of importing a specific class of the OCCT API is

from OCP.thePackageName import theClassName

For example if you want to use the class BRepPrimAPI_MakeBox. You will go by the following

from OCP.BRepPrimAPI import BRepPrimAPI_MakeBox

The package name of any class is written at the top of the documentation page. Often it’s written in the class name itself as a prefix.

Going back and forth between the APIs

While the 3 APIs provide 3 different layer of complexity and functionality you can mix the 3 layers as you wish. Below is presented the different ways you can interact with the different API layers.

Fluent API <=> Direct API

Here are all the possibilities you have to get an object from the Direct API (i.e a topological object).

You can end the Fluent API call chain and get the last object on the stack with Workplane.val() alternatively you can get all the objects with Workplane.vals()

>>> box = Workplane().box(10, 5, 5)
>>> print(type(box))
<class cadquery.cq.Workplane>

>>> box = Workplane().box(10, 5, 5).val()
>>> print(type(box))
<class cadquery.occ_impl.shapes.Solid>

If you are only interested in getting the context solid of your Workplane, you can use Workplane.findSolid():

>>> part = Workplane().box(10,5,5).circle(3).val()
>>> print(type(part))
<class cadquery.cq.Wire>

>>> part = Workplane().box(10,5,5).circle(3).findSolid()
>>> print(type(part))
<class cadquery.occ_impl.shapes.Compound>
# The return type of findSolid is either a Solid or a Compound object

If you want to go the other way around i.e using objects from the topological API in the Fluent API here are your options :

You can pass a topological object as a base object to the Workplane object.

solid_box = Solid.makeBox(10, 10, 10)
part = Workplane(obj=solid_box)
# And you can continue your modelling in the fluent API
part = part.faces(">Z").circle(1).extrude(10)

You can add a topological object as a new operation/step in the Fluent API call chain with Workplane.newObject()

circle_wire = Wire.makeCircle(1, Vector(0, 0, 0), Vector(0, 0, 1))
box = Workplane().box(10, 10, 10).newObject([circle_wire])
# And you can continue modelling
box = (
    box.toPending().cutThruAll()
)  # notice the call to `toPending` that is needed if you want to use it in a subsequent operation

Direct API <=> OCCT API

Every object of the Direct API stores its OCCT equivalent object in its wrapped attribute.:

>>> box = Solid.makeBox(10,5,5)
>>> print(type(box))
<class cadquery.occ_impl.shapes.Solid>

>>> box = Solid.makeBox(10,5,5).wrapped
>>> print(type(box))
<class OCP.TopoDS.TopoDS_Solid>

If you want to cast an OCCT object into a Direct API one you can just pass it as a parameter of the intended class:

>>> occt_box = BRepPrimAPI_MakeBox(5,5,5).Solid()
>>> print(type(occt_box))
<class OCP.TopoDS.TopoDS_Solid>

>>> direct_api_box = Solid(occt_box)
>>> print(type(direct_api_box))
<class cadquery.occ_impl.shapes.Solid>

Note

You can cast into the direct API the types found here

Multimethods

CadQuery uses Multimethod to allow a call to a method to be dispatched depending on the types of the arguments. An example is arc(), where a_sketch.arc((1, 2), (2, 3)) would be dispatched to one method but a_sketch.arc((1, 2), (2, 3), (3, 4)) would be dispatched to a different method. For multimethods to work, you should not use keyword arguments to specify positional parameters. For example, you should not write a_sketch.arc(p1=(1, 2), p2=(2, 3), p3=(3, 4)), instead you should use the previous example. Note CadQuery makes an attempt to fall back on the first registered multimethod in the event of a dispatch error, but it is still best practice to not use keyword arguments to specify positional arguments in CadQuery.

An Introspective Example

Note

If you are just beginning with CadQuery then you can leave this example for later. If you have some experience with creating CadQuery models and now you want to read the CadQuery source to better understand what your code does, then it is recommended you read this example first.

To demonstrate the above concepts, we can define more detailed string representations for the Workplane, Plane and CQContext classes and patch them in:

import cadquery as cq


def tidy_repr(obj):
    """Shortens a default repr string"""
    return repr(obj).split(".")[-1].rstrip(">")


def _ctx_str(self):
    return (
        tidy_repr(self)
        + ":\n"
        + f"    pendingWires: {self.pendingWires}\n"
        + f"    pendingEdges: {self.pendingEdges}\n"
        + f"    tags: {self.tags}"
    )


cq.cq.CQContext.__str__ = _ctx_str


def _plane_str(self):
    return (
        tidy_repr(self)
        + ":\n"
        + f"    origin: {self.origin.toTuple()}\n"
        + f"    z direction: {self.zDir.toTuple()}"
    )


cq.occ_impl.geom.Plane.__str__ = _plane_str


def _wp_str(self):
    out = tidy_repr(self) + ":\n"
    out += f"  parent: {tidy_repr(self.parent)}\n" if self.parent else "  no parent\n"
    out += f"  plane: {self.plane}\n"
    out += f"  objects: {self.objects}\n"
    out += f"  modelling context: {self.ctx}"
    return out


cq.Workplane.__str__ = _wp_str

Now we can make a simple part and examine the Workplane and CQContext objects at each step. The final part looks like:

part = (
    cq.Workplane()
    .box(1, 1, 1)
    .tag("base")
    .wires(">Z")
    .toPending()
    .translate((0.1, 0.1, 1.0))
    .toPending()
    .loft()
    .faces(">>X", tag="base")
    .workplane(centerOption="CenterOfMass")
    .circle(0.2)
    .extrude(1)
)

Note

Some of the modelling process for this part is a bit contrived and not a great example of fluent CadQuery techniques.

The start of our chain of calls is:

part = cq.Workplane()
print(part)

Which produces the output:

Workplane object at 0x2760:
  no parent
  plane: Plane object at 0x2850:
    origin: (0.0, 0.0, 0.0)
    z direction: (0.0, 0.0, 1.0)
  objects: []
  modelling context: CQContext object at 0x2730:
    pendingWires: []
    pendingEdges: []
    tags: {}

This is simply an empty Workplane. Being the first Workplane in the chain, it does not have a parent. The plane attribute contains a Plane object that describes the XY plane.

Now we create a simple box. To keep things short, the print(part) line will not be shown for the rest of these code blocks:

part = part.box(1, 1, 1)

Which produces the output:

Workplane object at 0xaa90:
  parent: Workplane object at 0x2760
  plane: Plane object at 0x3850:
    origin: (0.0, 0.0, 0.0)
    z direction: (0.0, 0.0, 1.0)
  objects: [<cadquery.occ_impl.shapes.Solid object at 0xbbe0>]
  modelling context: CQContext object at 0x2730:
    pendingWires: []
    pendingEdges: []
    tags: {}

The first thing to note is that this is a different Workplane object to the previous one, and in the parent attribute of this Workplane is our previous Workplane. Returning a new instance of Workplane is the normal behaviour of most Workplane methods (with some exceptions, as will be shown below) and this is how the chaining concept is implemented.

Secondly, the modelling context object is the same as the one in the previous Workplane, and this one modelling context at 0x2730 will be shared between every Workplane object in this chain. If we instantiate a new Workplane with part2 = cq.Workplane(), then this part2 would have a different instance of the CQContext attached to it.

Thirdly, in our objects list is a single Solid object, which is the box we just created.

Often when creating models you will find yourself wanting to refer back to a specific Workplane object, perhaps because it is easier to select the feature you want in this earlier state, or because you want to reuse a plane. Tags offer a way to refer back to a previous Workplane. We can tag the Workplane that contains this basic box now:

part = part.tag("base")

The string representation of part is now:

Workplane object at 0xaa90:
  parent: Workplane object at 0x2760
  plane: Plane object at 0x3850:
    origin: (0.0, 0.0, 0.0)
    z direction: (0.0, 0.0, 1.0)
  objects: [<cadquery.occ_impl.shapes.Solid object at 0xbbe0>]
  modelling context: CQContext object at 0x2730:
    pendingWires: []
    pendingEdges: []
    tags: {'base': <cadquery.cq.Workplane object at 0xaa90>}

The tags attribute of the modelling context is simply a dict associating the string name given by the tag() method to the Workplane. Methods such as workplaneFromTagged() and selection methods like edges() can operate on a tagged Workplane. Note that unlike the part = part.box(1, 1, 1) step where we went from Workplane object at 0x2760 to Workplane object at 0xaa90, the tag() method has returned the same object at 0xaa90. This is unusual for a Workplane method.

The next step is:

part = part.faces(">>Z")

The output is:

Workplane object at 0x8c40:
  parent: Workplane object at 0xaa90
  plane: Plane object at 0xac40:
    origin: (0.0, 0.0, 0.0)
    z direction: (0.0, 0.0, 1.0)
  objects: [<cadquery.occ_impl.shapes.Face object at 0x3c10>]
  modelling context: CQContext object at 0x2730:
    pendingWires: []
    pendingEdges: []
    tags: {'base': <cadquery.cq.Workplane object at 0xaa90>}

Our selection method has taken the Solid from the objects list of the previous Workplane, found the face with it’s center furthest in the Z direction, and placed that face into the objects attribute. The Solid representing the box we are modelling is gone, and when a Workplane method needs to access that solid it searches through the parent chain for the nearest solid. This action can also be done by a user through the findSolid() method.

Now we want to select the boundary of this Face (a Wire), so we use:

part = part.wires()

The output is now:

Workplane object at 0x6880:
  parent: Workplane object at 0x8c40
  plane: Plane object at 0x38b0:
    origin: (0.0, 0.0, 0.0)
    z direction: (0.0, 0.0, 1.0)
  objects: [<cadquery.occ_impl.shapes.Wire object at 0xaca0>]
  modelling context: CQContext object at 0x2730:
    pendingWires: []
    pendingEdges: []
    tags: {'base': <cadquery.cq.Workplane object at 0xaa90>}

Modelling operations take their wires and edges from the modelling context’s pending lists. In order to use the loft() command further down the chain, we need to push this wire to the modelling context with:

part = part.toPending()

Now we have:

Workplane object at 0x6880:
  parent: Workplane object at 0x8c40
  plane: Plane object at 0x38b0:
    origin: (0.0, 0.0, 0.0)
    z direction: (0.0, 0.0, 1.0)
  objects: [<cadquery.occ_impl.shapes.Wire object at 0xaca0>]
  modelling context: CQContext object at 0x2730:
    pendingWires: [<cadquery.occ_impl.shapes.Wire object at 0xaca0>]
    pendingEdges: []
    tags: {'base': <cadquery.cq.Workplane object at 0xaa90>}

The Wire object that was only in the objects attribute before is now also in the modelling context’s pendingWires. The toPending() method is also another of the unusual methods that return the same Workplane object instead of a new one.

To set up the other side of the loft() command further down the chain, we translate the wire in objects by calling:

part = part.translate((0.1, 0.1, 1.0))

Now the string representation of part looks like:

Workplane object at 0x3a00:
  parent: Workplane object at 0x6880
  plane: Plane object at 0xac70:
    origin: (0.0, 0.0, 0.0)
    z direction: (0.0, 0.0, 1.0)
  objects: [<cadquery.occ_impl.shapes.Wire object at 0x35e0>]
  modelling context: CQContext object at 0x2730:
    pendingWires: [<cadquery.occ_impl.shapes.Wire object at 0xaca0>]
    pendingEdges: []
    tags: {'base': <cadquery.cq.Workplane object at 0xaa90>}

It may look similar to the previous step, but the Wire object in objects is different. To get this wire into the pending wires list, again we use:

part = part.toPending()

The result:

Workplane object at 0x3a00:
  parent: Workplane object at 0x6880
  plane: Plane object at 0xac70:
    origin: (0.0, 0.0, 0.0)
    z direction: (0.0, 0.0, 1.0)
  objects: [<cadquery.occ_impl.shapes.Wire object at 0x35e0>]
  modelling context: CQContext object at 0x2730:
    pendingWires: [<cadquery.occ_impl.shapes.Wire object at 0xaca0>, <cadquery.occ_impl.shapes.Wire object at 0x7f5c7f5c35e0>]
    pendingEdges: []
    tags: {'base': <cadquery.cq.Workplane object at 0xaa90>}

The modelling context’s pendingWires attribute now contains the two wires we want to loft between, and we simply call:

part = part.loft()

After the loft operation, our Workplane looks quite different:

Workplane object at 0x32b0:
  parent: Workplane object at 0x3a00
  plane: Plane object at 0x3d60:
    origin: (0.0, 0.0, 0.0)
    z direction: (0.0, 0.0, 1.0)
  objects: [<cadquery.occ_impl.shapes.Compound object at 0xad30>]
  modelling context: CQContext object at 0x2730:
    pendingWires: []
    pendingEdges: []
    tags: {'base': <cadquery.cq.Workplane object at 0xaa90>}

In the cq.Workplane.objects attribute we now have one Compound object and the modelling context’s pendingWires has been cleared by loft().

Note

To inspect the Compound object further you can use val() or findSolid() to get at the Compound object, then use cadquery.Shape.Solids() to return a list of the Solid objects contained in the Compound, which in this example will be a single Solid object. For example:

>>> a_compound = part.findSolid()
>>> a_list_of_solids = a_compound.Solids()
>>> len(a_list_of_solids)
1

Now we will create a small cylinder protruding from a face on the original box. We need to set up a workplane to draw a circle on, so firstly we will select the correct face:

part = part.faces(">>X", tag="base")

Which results in:

Workplane object at 0x3f10:
  parent: Workplane object at 0x32b0
  plane: Plane object at 0xefa0:
    origin: (0.0, 0.0, 0.0)
    z direction: (0.0, 0.0, 1.0)
  objects: [<cadquery.occ_impl.shapes.Face object at 0x3af0>]
  modelling context: CQContext object at 0x2730:
    pendingWires: []
    pendingEdges: []
    tags: {'base': <cadquery.cq.Workplane object at 0xaa90>}

We have the desired Face in the objects attribute, but the plane has not changed yet. To create the new plane we use the Workplane.workplane() method:

part = part.workplane()

Now:

Workplane object at 0xe700:
  parent: Workplane object at 0x3f10
  plane: Plane object at 0xe730:
    origin: (0.5, 0.0, 0.0)
    z direction: (1.0, 0.0, 0.0)
  objects: []
  modelling context: CQContext object at 0x2730:
    pendingWires: []
    pendingEdges: []
    tags: {'base': <cadquery.cq.Workplane object at 0xaa90>}

The objects list has been cleared and the Plane object has a local Z direction in the global X direction. Since the base of the plane is the side of the box, the origin is offset in the X direction.

Onto this plane we can draw a circle:

part = part.circle(0.2)

Now:

Workplane object at 0xe790:
  parent: Workplane object at 0xe700
  plane: Plane object at 0xaf40:
    origin: (0.5, 0.0, 0.0)
    z direction: (1.0, 0.0, 0.0)
  objects: [<cadquery.occ_impl.shapes.Wire object at 0xe610>]
  modelling context: CQContext object at 0x2730:
    pendingWires: [<cadquery.occ_impl.shapes.Wire object at 0xe610>]
    pendingEdges: []
    tags: {'base': <cadquery.cq.Workplane object at 0xaa90>}

The circle() method - like all 2D drawing methods - has placed the circle into both the objects attribute (where it will be cleared during the next modelling step), and the modelling context’s pending wires (where it will persist until used by another Workplane method).

The next step is to extrude this circle and create a cylindrical protrusion:

part = part.extrude(1, clean=False)

Now:

Workplane object at 0xafd0:
  parent: Workplane object at 0xe790
  plane: Plane object at 0x3e80:
    origin: (0.5, 0.0, 0.0)
    z direction: (1.0, 0.0, 0.0)
  objects: [<cadquery.occ_impl.shapes.Compound object at 0xaaf0>]
  modelling context: CQContext object at 0x2730:
    pendingWires: []
    pendingEdges: []
    tags: {'base': <cadquery.cq.Workplane object at 0xaa90>}

The extrude() method has cleared all the pending wires and edges. The objects attribute contains the final Compound object that is shown in the 3D view above.

Note

The extrude() has an argument for clean which defaults to True. This extrudes the pending wires (creating a new Workplane object), then runs the clean() method to refine the result, creating another Workplane. If you were to run the example with the default clean=True then you would see an intermediate Workplane object in parent rather than the object from the previous step.

Assemblies

Simple models can be combined into complex, possibly nested, assemblies.

A simple example could look as follows:

from cadquery import *

w = 10
d = 10
h = 10

part1 = Workplane().box(2 * w, 2 * d, h)
part2 = Workplane().box(w, d, 2 * h)
part3 = Workplane().box(w, d, 3 * h)

assy = (
    Assembly(part1, loc=Location(Vector(-w, 0, h / 2)))
    .add(
        part2, loc=Location(Vector(1.5 * w, -0.5 * d, h / 2)), color=Color(0, 0, 1, 0.5)
    )
    .add(part3, loc=Location(Vector(-0.5 * w, -0.5 * d, 2 * h)), color=Color("red"))
)

Resulting in:

Note that the locations of the children parts are defined with respect to their parents - in the above example part3 will be located at (-5,-5,20) in the global coordinate system. Assemblies with different colors can be created this way and exported to STEP or the native OCCT xml format.

You can browse assembly related methods here: Assemblies.

Assemblies with constraints

Sometimes it is not desirable to define the component positions explicitly but rather use constraints to obtain a fully parametric assembly. This can be achieved in the following way:

from cadquery import *

w = 10
d = 10
h = 10

part1 = Workplane().box(2 * w, 2 * d, h)
part2 = Workplane().box(w, d, 2 * h)
part3 = Workplane().box(w, d, 3 * h)

assy = (
    Assembly(part1, name="part1", loc=Location(Vector(-w, 0, h / 2)))
    .add(part2, name="part2", color=Color(0, 0, 1, 0.5))
    .add(part3, name="part3", color=Color("red"))
    .constrain("part1@faces@>Z", "part3@faces@<Z", "Axis")
    .constrain("part1@faces@>Z", "part2@faces@<Z", "Axis")
    .constrain("part1@faces@>Y", "part3@faces@<Y", "Axis")
    .constrain("part1@faces@>Y", "part2@faces@<Y", "Axis")
    .constrain("part1@vertices@>(-1,-1,1)", "part3@vertices@>(-1,-1,-1)", "Point")
    .constrain("part1@vertices@>(1,-1,-1)", "part2@vertices@>(-1,-1,-1)", "Point")
    .solve()
)

This code results in identical object as one from the previous section. The added benefit is that with changing parameters w, d, h the final locations will be calculated automatically. It is admittedly dense and can be made clearer using tags. Tags can be directly referenced when constructing the constraints:

from cadquery import *

w = 10
d = 10
h = 10

part1 = Workplane().box(2 * w, 2 * d, h)
part2 = Workplane().box(w, d, 2 * h)
part3 = Workplane().box(w, d, 3 * h)

part1.faces(">Z").edges("<X").vertices("<Y").tag("pt1")
part1.faces(">X").edges("<Z").vertices("<Y").tag("pt2")
part3.faces("<Z").edges("<X").vertices("<Y").tag("pt1")
part2.faces("<X").edges("<Z").vertices("<Y").tag("pt2")

assy1 = (
    Assembly(part1, name="part1", loc=Location(Vector(-w, 0, h / 2)))
    .add(part2, name="part2", color=Color(0, 0, 1, 0.5))
    .add(part3, name="part3", color=Color("red"))
    .constrain("part1@faces@>Z", "part3@faces@<Z", "Axis")
    .constrain("part1@faces@>Z", "part2@faces@<Z", "Axis")
    .constrain("part1@faces@>Y", "part3@faces@<Y", "Axis")
    .constrain("part1@faces@>Y", "part2@faces@<Y", "Axis")
    .constrain("part1?pt1", "part3?pt1", "Point")
    .constrain("part1?pt2", "part2?pt2", "Point")
    .solve()
)

The following constraints are currently implemented:

Axis

two normal vectors are anti-coincident or the angle (in radians) between them is equal to the specified value. Can be defined for all entities with consistent normal vector - planar faces, wires and edges.

Point

two points are coincident or separated by a specified distance. Can be defined for all entities, center of mass is used for lines, faces, solids and the vertex position for vertices.

Plane

combination of :Axis: and :Point: constraints.

For a more elaborate assembly example see Assemblies.