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):
a single point in space
a connection between two or more vertices along a particular path (called a curve)
a collection of edges that are connected together.
a set of edges or wires that enclose a surface
a collection of faces that are connected together along some of their edges
a shell that has a closed interior
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.
CQ, the CadQuery Object¶
The CadQuery object wraps a BREP feature, and provides functionality around it. Typical examples include rotating, transforming, combining objects, and creating workplanes.
See CadQuery API Reference to learn more.
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.
cadquery.Workplane to learn more.
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 2-d Operations to learn more.
You can construct 3D primitives such as boxes, spheres, wedges, and cylinders directly. You can also sweep, extrude, and loft 2D geometry to form 3D features. Of course the basic primitive operations are also available.
See 3-d Operations to learn more.
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.
You can learn more about selectors Selectors
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
As you work in CadQuery, each operation returns a new CadQuery object with the result of that operations. Each CadQuery 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:
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:
You can browse stack access methods here: Stack and Selector Methods.
All CadQuery methods return another CadQuery object, so that you can chain the methods together fluently. Use the core CQ methods to get at the objects that were created.
Each time a new CadQuery object is produced during these chained calls, it has a
parent attribute that points
to the CadQuery object that created it. Several CadQuery methods search this parent chain, for example when searching
for the context solid. You can also give a CadQuery object a tag, and further down your chain of CadQuery 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:
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.
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:
Will actually create 4 circles, because
vertices() selects 4 vertices of a rectangular face, and the
iterates on each member of the stack.
This is really useful to remember when you author your own plugins.
cadquery.cq.Workplane.each() is useful for this purpose.
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,-.5*d,h/2)), color=Color(0,0,1,0.5)) .add(part3, loc=Location(Vector(-.5*w,-.5*d,2*h)), color=Color("red")) )
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
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:
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.
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.
combination of :Axis: and :Point: constraints.
For a more elaborate assembly example see Assembly Tutorial.