CadQuery Class Summary

This page documents all of the methods and functions of the CadQuery classes, organized alphabetically.

See also

For a listing organized by functional area, see the API Reference

Core Classes

Sketch(parent, locs, obj)

2D sketch.

Workplane(, obj=None))

Defines a coordinate system in space, in which 2D coordinates can be used.

Assembly([obj, loc, name, color, metadata])

Nested assembly of Workplane and Shape objects defining their relative positions.

Constraint

alias of ConstraintSpec

Topological Classes

Shape(obj)

Represents a shape in the system.

Vertex(obj[, forConstruction])

A Single Point in Space

Edge(obj)

A trimmed curve that represents the border of a face

cadquery.occ_impl.shapes.Mixin1D()

Wire(obj)

A series of connected, ordered Edges, that typically bounds a Face

Face(obj)

a bounded surface that represents part of the boundary of a solid

Shell(obj)

the outer boundary of a surface

cadquery.occ_impl.shapes.Mixin3D()

Solid(obj)

a single solid

Compound(obj)

a collection of disconnected solids

Geometry Classes

Vector()

Create a 3-dimensional vector

Matrix()

A 3d , 4x4 transformation matrix.

Plane(origin[, xDir, normal])

A 2D coordinate system in space

Location(t)

Location in 3D space.

Selector Classes

Selector()

Filters a list of objects.

NearestToPointSelector(pnt)

Selects object nearest the provided point.

BoxSelector(point0, point1[, boundingbox])

Selects objects inside the 3D box defined by 2 points.

BaseDirSelector(vector[, tolerance])

A selector that handles selection on the basis of a single direction vector.

ParallelDirSelector(vector[, tolerance])

Selects objects parallel with the provided direction.

DirectionSelector(vector[, tolerance])

Selects objects aligned with the provided direction.

PerpendicularDirSelector(vector[, tolerance])

Selects objects perpendicular with the provided direction.

TypeSelector(typeString)

Selects objects having the prescribed geometry type.

RadiusNthSelector(n[, directionMax, tolerance])

Select the object with the Nth radius.

CenterNthSelector(vector, n[, directionMax, ...])

Sorts objects into a list with order determined by the distance of their center projected onto the specified direction.

DirectionMinMaxSelector(vector[, ...])

Selects objects closest or farthest in the specified direction.

DirectionNthSelector(vector, n[, ...])

Filters for objects parallel (or normal) to the specified direction then returns the Nth one.

LengthNthSelector(n[, directionMax, tolerance])

Select the object(s) with the Nth length

AreaNthSelector(n[, directionMax, tolerance])

Selects the object(s) with Nth area

BinarySelector(left, right)

Base class for selectors that operates with two other selectors.

AndSelector(left, right)

Intersection selector.

SumSelector(left, right)

Union selector.

SubtractSelector(left, right)

Difference selector.

InverseSelector(selector)

Inverts the selection of given selector.

StringSyntaxSelector(selectorString)

Filter lists objects using a simple string syntax.

Class Details

class cadquery.Assembly(obj: Optional[Union[Shape, Workplane]] = None, loc: Optional[Location] = None, name: Optional[str] = None, color: Optional[Color] = None, metadata: Optional[Dict[str, Any]] = None)[source]

Bases: object

Nested assembly of Workplane and Shape objects defining their relative positions.

Parameters

  • obj (Optional[Union[Shape, Workplane]]) –

  • loc (Location) –

  • name (str) –

  • color (Optional[Color]) –

  • metadata (Dict[str, Any]) –

__init__(obj: Optional[Union[Shape, Workplane]] = None, loc: Optional[Location] = None, name: Optional[str] = None, color: Optional[Color] = None, metadata: Optional[Dict[str, Any]] = None)[source]

construct an assembly

Parameters

  • obj (Optional[Union[Shape, Workplane]]) – root object of the assembly (default: None)

  • loc (Optional[Location]) – location of the root object (default: None, interpreted as identity transformation)

  • name (Optional[str]) – unique name of the root object (default: None, resulting in an UUID being generated)

  • color (Optional[Color]) – color of the added object (default: None)

  • metadata (Optional[Dict[str, Any]]) – a store for user-defined metadata (default: None)

Returns

An Assembly object.

To create an empty assembly use:

assy = Assembly(None)

To create one constraint a root object:

b = Workplane().box(1, 1, 1)
assy = Assembly(b, Location(Vector(0, 0, 1)), name="root")
__iter__(loc: Optional[Location] = None, name: Optional[str] = None, color: Optional[Color] = None) → Iterator[Tuple[Shape, str, Location, Optional[Color]]][source]

Assembly iterator yielding shapes, names, locations and colors.

Parameters

  • loc (Optional[Location]) –

  • name (Optional[str]) –

  • color (Optional[Color]) –

Return type

Iterator[Tuple[Shape, str, Location, Optional[Color]]]

__weakref__

list of weak references to the object (if defined)

add(obj: Assembly, loc: Optional[Location] = None, name: Optional[str] = None, color: Optional[Color] = None) → Assembly[source]
add(obj: Optional[Union[Shape, Workplane]], loc: Optional[Location] = None, name: Optional[str] = None, color: Optional[Color] = None, metadata: Optional[Dict[str, Any]] = None) → Assembly

Add a subassembly to the current assembly.

constrain(q1: str, q2: str, kind: Literal['Plane', 'Point', 'Axis', 'PointInPlane', 'Fixed', 'FixedPoint', 'FixedAxis', 'PointOnLine', 'FixedRotation'], param: Any = None) → Assembly[source]
constrain(q1: str, kind: Literal['Plane', 'Point', 'Axis', 'PointInPlane', 'Fixed', 'FixedPoint', 'FixedAxis', 'PointOnLine', 'FixedRotation'], param: Any = None) → Assembly
constrain(id1: str, s1: Shape, id2: str, s2: Shape, kind: Literal['Plane', 'Point', 'Axis', 'PointInPlane', 'Fixed', 'FixedPoint', 'FixedAxis', 'PointOnLine', 'FixedRotation'], param: Any = None) → Assembly
constrain(id1: str, s1: Shape, kind: Literal['Plane', 'Point', 'Axis', 'PointInPlane', 'Fixed', 'FixedPoint', 'FixedAxis', 'PointOnLine', 'FixedRotation'], param: Any = None) → Assembly

Define a new constraint.

export(path: str, exportType: Optional[Literal['STEP', 'XML', 'GLTF', 'VTKJS', 'VRML', 'STL']] = None, mode: Literal['default', 'fused'] = 'default', tolerance: float = 0.1, angularTolerance: float = 0.1, **kwargs) → Assembly[source]

Save assembly to a file.

Parameters

  • path (str) – Path and filename for writing.

  • exportType (Optional[Literal['STEP', 'XML', 'GLTF', 'VTKJS', 'VRML', 'STL']]) – export format (default: None, results in format being inferred form the path)

  • mode (Literal['default', 'fused']) – STEP only - See exportAssembly().

  • tolerance (float) – the deflection tolerance, in model units. Only used for glTF, VRML. Default 0.1.

  • angularTolerance (float) – the angular tolerance, in radians. Only used for glTF, VRML. Default 0.1.

  • **kwargs – Additional keyword arguments. Only used for STEP, glTF and STL. See exportAssembly().

  • ascii (bool) – STL only - Sets whether or not STL export should be text or binary

Return type

Assembly

save(path: str, exportType: Optional[Literal['STEP', 'XML', 'GLTF', 'VTKJS', 'VRML', 'STL']] = None, mode: Literal['default', 'fused'] = 'default', tolerance: float = 0.1, angularTolerance: float = 0.1, **kwargs) → Assembly[source]

Save assembly to a file.

Parameters

  • path (str) – Path and filename for writing.

  • exportType (Optional[Literal['STEP', 'XML', 'GLTF', 'VTKJS', 'VRML', 'STL']]) – export format (default: None, results in format being inferred form the path)

  • mode (Literal['default', 'fused']) – STEP only - See exportAssembly().

  • tolerance (float) – the deflection tolerance, in model units. Only used for glTF, VRML. Default 0.1.

  • angularTolerance (float) – the angular tolerance, in radians. Only used for glTF, VRML. Default 0.1.

  • **kwargs – Additional keyword arguments. Only used for STEP, glTF and STL. See exportAssembly().

  • ascii (bool) – STL only - Sets whether or not STL export should be text or binary

Return type

Assembly

property shapes: List[Shape]

List of Shape objects in the .obj field

solve(verbosity: int = 0) → Assembly[source]

Solve the constraints.

Parameters

verbosity (int) –

Return type

Assembly

toCompound() → Compound[source]

Returns a Compound made from this Assembly (including all children) with the current Locations applied. Usually this method would only be used after solving.

Return type

Compound

traverse() → Iterator[Tuple[str, Assembly]][source]

Yield (name, child) pairs in a bottom-up manner

Return type

Iterator[Tuple[str, Assembly]]

class cadquery.BoundBox(bb: Bnd_Box)[source]

Bases: object

A BoundingBox for an object or set of objects. Wraps the OCP one

Parameters

bb (Bnd_Box) –

__init__(bb: Bnd_Box) → None[source]
Parameters

bb (Bnd_Box) –

Return type

None

__weakref__

list of weak references to the object (if defined)

add(obj: Union[Tuple[float, float, float], Vector, BoundBox], tol: Optional[float] = None) → BoundBox[source]

Returns a modified (expanded) bounding box

obj can be one of several things:

  1. a 3-tuple corresponding to x,y, and z amounts to add

  2. a vector, containing the x,y,z values to add

  3. another bounding box, where a new box will be created that encloses both.

This bounding box is not changed.

Parameters

  • obj (Union[Tuple[float, float, float], Vector, BoundBox]) –

  • tol (Optional[float]) –

Return type

BoundBox

enlarge(tol: float) → BoundBox[source]

Returns a modified (expanded) bounding box, expanded in all directions by the tolerance value.

This means that the minimum values of its X, Y and Z intervals of the bounding box are reduced by the absolute value of tol, while the maximum values are increased by the same amount.

Parameters

tol (float) –

Return type

BoundBox

static findOutsideBox2D(bb1: BoundBox, bb2: BoundBox) → Optional[BoundBox][source]

Compares bounding boxes

Compares bounding boxes. Returns none if neither is inside the other. Returns the outer one if either is outside the other.

BoundBox.isInside works in 3d, but this is a 2d bounding box, so it doesn’t work correctly plus, there was all kinds of rounding error in the built-in implementation i do not understand.

Parameters
Return type

Optional[BoundBox]

isInside(b2: BoundBox) → bool[source]

Is the provided bounding box inside this one?

Parameters

b2 (BoundBox) –

Return type

bool

cadquery.CQ

alias of Workplane

class cadquery.Color(name: str)[source]
class cadquery.Color(r: float, g: float, b: float, a: float = 0)
class cadquery.Color

Bases: object

Wrapper for the OCCT color object Quantity_ColorRGBA.

__init__(name: str)[source]
__init__(r: float, g: float, b: float, a: float = 0)
__init__()
__weakref__

list of weak references to the object (if defined)

toTuple() → Tuple[float, float, float, float][source]

Convert Color to RGB tuple.

Return type

Tuple[float, float, float, float]

class cadquery.Compound(obj: TopoDS_Shape)[source]

Bases: Shape, Mixin3D

a collection of disconnected solids

Parameters

obj (TopoDS_Shape) –

__bool__() → bool[source]

Check if empty.

Return type

bool

ancestors(shape: Shape, kind: Literal['Vertex', 'Edge', 'Wire', 'Face', 'Shell', 'Solid', 'CompSolid', 'Compound']) → Compound[source]

Iterate over ancestors, i.e. shapes of same kind within shape that contain elements of self.

Parameters

  • shape (Shape) –

  • kind (Literal['Vertex', 'Edge', 'Wire', 'Face', 'Shell', 'Solid', 'CompSolid', 'Compound']) –

Return type

Compound

cut(*toCut: Shape, tol: Optional[float] = None) → Compound[source]

Remove the positional arguments from this Shape.

Parameters

  • tol (Optional[float]) – Fuzzy mode tolerance

  • toCut (Shape) –

Return type

Compound

fuse(*toFuse: Shape, glue: bool = False, tol: Optional[float] = None) → Compound[source]

Fuse shapes together

Parameters

  • toFuse (Shape) –

  • glue (bool) –

  • tol (Optional[float]) –

Return type

Compound

intersect(*toIntersect: Shape, tol: Optional[float] = None) → Compound[source]

Intersection of the positional arguments and this Shape.

Parameters

  • tol (Optional[float]) – Fuzzy mode tolerance

  • toIntersect (Shape) –

Return type

Compound

classmethod makeCompound(listOfShapes: Iterable[Shape]) → Compound[source]

Create a compound out of a list of shapes

Parameters

listOfShapes (Iterable[Shape]) –

Return type

Compound

classmethod makeText(text: str, size: float, height: float, font: str = 'Arial', fontPath: Optional[str] = None, kind: Literal['regular', 'bold', 'italic'] = 'regular', halign: Literal['center', 'left', 'right'] = 'center', valign: Literal['center', 'top', 'bottom'] = 'center', position: Plane = Plane(origin=(0.0, 0.0, 0.0), xDir=(1.0, 0.0, 0.0), normal=(0.0, 0.0, 1.0))) → Shape[source]

Create a 3D text

Parameters

  • text (str) –

  • size (float) –

  • height (float) –

  • font (str) –

  • fontPath (Optional[str]) –

  • kind (Literal['regular', 'bold', 'italic']) –

  • halign (Literal['center', 'left', 'right']) –

  • valign (Literal['center', 'top', 'bottom']) –

  • position (Plane) –

Return type

Shape

remove(shape: Shape)[source]

Remove the specified shape.

Parameters

shape (Shape) –

siblings(shape: Shape, kind: Literal['Vertex', 'Edge', 'Wire', 'Face', 'Shell', 'Solid', 'CompSolid', 'Compound'], level: int = 1) → Compound[source]

Iterate over siblings, i.e. shapes within shape that share subshapes of kind with the elements of self.

Parameters

  • shape (Shape) –

  • kind (Literal['Vertex', 'Edge', 'Wire', 'Face', 'Shell', 'Solid', 'CompSolid', 'Compound']) –

  • level (int) –

Return type

Compound

cadquery.Constraint

alias of ConstraintSpec

class cadquery.DirectionMinMaxSelector(vector: Vector, directionMax: bool = True, tolerance: float = 0.0001)[source]

Bases: CenterNthSelector

Selects objects closest or farthest in the specified direction.

Applicability:

All object types. for a vertex, its point is used. for all other kinds of objects, the center of mass of the object is used.

You can use the string shortcuts >(X|Y|Z) or <(X|Y|Z) if you want to select based on a cardinal direction.

For example this:

CQ(aCube).faces(DirectionMinMaxSelector((0, 0, 1), True))

Means to select the face having the center of mass farthest in the positive z direction, and is the same as:

CQ(aCube).faces(">Z")
Parameters

  • vector (Vector) –

  • directionMax (bool) –

  • tolerance (float) –

__init__(vector: Vector, directionMax: bool = True, tolerance: float = 0.0001)[source]
Parameters

  • vector (Vector) –

  • directionMax (bool) –

  • tolerance (float) –

class cadquery.DirectionSelector(vector: Vector, tolerance: float = 0.0001)[source]

Bases: BaseDirSelector

Selects objects aligned with the provided direction.

Applicability:

Linear Edges Planar Faces

Use the string syntax shortcut +/-(X|Y|Z) if you want to select based on a cardinal direction.

Example:

CQ(aCube).faces(DirectionSelector((0, 0, 1)))

selects faces with the normal in the z direction, and is equivalent to:

CQ(aCube).faces("+Z")
Parameters

  • vector (Vector) –

  • tolerance (float) –

test(vec: Vector) → bool[source]

Test a specified vector. Subclasses override to provide other implementations

Parameters

vec (Vector) –

Return type

bool

class cadquery.Edge(obj: TopoDS_Shape)[source]

Bases: Shape, Mixin1D

A trimmed curve that represents the border of a face

Parameters

obj (TopoDS_Shape) –

arcCenter() → Vector[source]

Center of an underlying circle or ellipse geometry.

Return type

Vector

close() → Union[Edge, Wire][source]

Close an Edge

Return type

Union[Edge, Wire]

classmethod makeBezier(points: List[Vector]) → Edge[source]

Create a cubic Bézier Curve from the points.

Parameters

points (List[Vector]) – a list of Vectors that represent the points. The edge will pass through the first and the last point, and the inner points are Bézier control points.

Returns

An edge

Return type

Edge

classmethod makeEllipse(x_radius: float, y_radius: float, pnt: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 0.0), dir: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 1.0), xdir: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (1.0, 0.0, 0.0), angle1: float = 360.0, angle2: float = 360.0, sense: ~typing.Literal[-1, 1] = 1) → Edge[source]

Makes an Ellipse centered at the provided point, having normal in the provided direction.

Parameters

  • cls –

  • x_radius (float) – x radius of the ellipse (along the x-axis of plane the ellipse should lie in)

  • y_radius (float) – y radius of the ellipse (along the y-axis of plane the ellipse should lie in)

  • pnt (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – vector representing the center of the ellipse

  • dir (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – vector representing the direction of the plane the ellipse should lie in

  • angle1 (float) – start angle of arc

  • angle2 (float) – end angle of arc (angle2 == angle1 return closed ellipse = default)

  • sense (Literal[-1, 1]) – clockwise (-1) or counter clockwise (1)

  • xdir (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

Returns

an Edge

Return type

Edge

classmethod makeLine(v1: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], v2: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → Edge[source]

Create a line between two points

Parameters

  • v1 (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – Vector that represents the first point

  • v2 (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – Vector that represents the second point

Returns

A linear edge between the two provided points

Return type

Edge

classmethod makeSpline(listOfVector: List[Vector], tangents: Optional[Sequence[Vector]] = None, periodic: bool = False, parameters: Optional[Sequence[float]] = None, scale: bool = True, tol: float = 1e-06) → Edge[source]

Interpolate a spline through the provided points.

Parameters

  • listOfVector (List[Vector]) – a list of Vectors that represent the points

  • tangents (Optional[Sequence[Vector]]) – tuple of Vectors specifying start and finish tangent

  • periodic (bool) – creation of periodic curves

  • parameters (Optional[Sequence[float]]) – the value of the parameter at each interpolation point. (The interpolated curve is represented as a vector-valued function of a scalar parameter.) If periodic == True, then len(parameters) must be len(intepolation points) + 1, otherwise len(parameters) must be equal to len(interpolation points).

  • scale (bool) – whether to scale the specified tangent vectors before interpolating. Each tangent is scaled, so it’s length is equal to the derivative of the Lagrange interpolated curve. I.e., set this to True, if you want to use only the direction of the tangent vectors specified by tangents, but not their magnitude.

  • tol (float) – tolerance of the algorithm (consult OCC documentation). Used to check that the specified points are not too close to each other, and that tangent vectors are not too short. (In either case interpolation may fail.)

Returns

an Edge

Return type

Edge

classmethod makeSplineApprox(listOfVector: List[Vector], tol: float = 0.001, smoothing: Optional[Tuple[float, float, float]] = None, minDeg: int = 1, maxDeg: int = 6) → Edge[source]

Approximate a spline through the provided points.

Parameters

  • listOfVector (List[Vector]) – a list of Vectors that represent the points

  • tol (float) – tolerance of the algorithm (consult OCC documentation).

  • smoothing (Optional[Tuple[float, float, float]]) – optional tuple of 3 weights use for variational smoothing (default: None)

  • minDeg (int) – minimum spline degree. Enforced only when smothing is None (default: 1)

  • maxDeg (int) – maximum spline degree (default: 6)

Returns

an Edge

Return type

Edge

classmethod makeTangentArc(v1: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], v2: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], v3: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → Edge[source]

Makes a tangent arc from point v1, in the direction of v2 and ends at v3.

Parameters

  • cls –

  • v1 (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – start vector

  • v2 (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – tangent vector

  • v3 (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – end vector

Returns

an edge

Return type

Edge

classmethod makeThreePointArc(v1: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], v2: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], v3: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → Edge[source]

Makes a three point arc through the provided points

Parameters

  • cls –

  • v1 (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – start vector

  • v2 (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – middle vector

  • v3 (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – end vector

Returns

an edge object through the three points

Return type

Edge

class cadquery.Face(obj: TopoDS_Shape)[source]

Bases: Shape

a bounded surface that represents part of the boundary of a solid

Parameters

obj (TopoDS_Shape) –

Center() → Vector[source]
Returns

The point of the center of mass of this Shape

Return type

Vector

chamfer2D(d: float, vertices: Iterable[Vertex]) → Face[source]

Apply 2D chamfer to a face

Parameters

  • d (float) –

  • vertices (Iterable[Vertex]) –

Return type

Face

fillet2D(radius: float, vertices: Iterable[Vertex]) → Face[source]

Apply 2D fillet to a face

Parameters

  • radius (float) –

  • vertices (Iterable[Vertex]) –

Return type

Face

classmethod makeFromWires(outerWire: Wire, innerWires: List[Wire] = []) → Face[source]

Makes a planar face from one or more wires

Parameters

  • outerWire (Wire) –

  • innerWires (List[Wire]) –

Return type

Face

classmethod makeNSidedSurface(edges: ~typing.Iterable[~typing.Union[~cadquery.occ_impl.shapes.Edge, ~cadquery.occ_impl.shapes.Wire]], constraints: ~typing.Iterable[~typing.Union[~cadquery.occ_impl.shapes.Edge, ~cadquery.occ_impl.shapes.Wire, ~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]], ~OCP.gp.gp_Pnt]], continuity: ~OCP.GeomAbs.GeomAbs_Shape = <GeomAbs_Shape.GeomAbs_C0: 0>, degree: int = 3, nbPtsOnCur: int = 15, nbIter: int = 2, anisotropy: bool = False, tol2d: float = 1e-05, tol3d: float = 0.0001, tolAng: float = 0.01, tolCurv: float = 0.1, maxDeg: int = 8, maxSegments: int = 9) → Face[source]

Returns a surface enclosed by a closed polygon defined by ‘edges’ and ‘constraints’.

Parameters

  • edges (list of edges or wires) – edges

  • constraints (list of points or edges) – constraints

  • continuity (GeomAbs_Shape) – OCC.Core.GeomAbs continuity condition

  • degree (int) – >=2

  • nbPtsOnCur (int) – number of points on curve >= 15

  • nbIter (int) – number of iterations >= 2

  • anisotropy (bool) – bool Anisotropy

  • tol2d (float) – 2D tolerance >0

  • tol3d (float) – 3D tolerance >0

  • tolAng (float) – angular tolerance

  • tolCurv (float) – tolerance for curvature >0

  • maxDeg (int) – highest polynomial degree >= 2

  • maxSegments (int) – greatest number of segments >= 2

Return type

Face

classmethod makeRuledSurface(edgeOrWire1: Edge, edgeOrWire2: Edge) → Face[source]
classmethod makeRuledSurface(edgeOrWire1: Wire, edgeOrWire2: Wire) → Face

makeRuledSurface(Edge|Wire,Edge|Wire) – Make a ruled surface Create a ruled surface out of two edges or wires. If wires are used then these must have the same number of edges

classmethod makeSplineApprox(points: List[List[Vector]], tol: float = 0.01, smoothing: Optional[Tuple[float, float, float]] = None, minDeg: int = 1, maxDeg: int = 3) → Face[source]

Approximate a spline surface through the provided points.

Parameters

  • points (List[List[Vector]]) – a 2D list of Vectors that represent the points

  • tol (float) – tolerance of the algorithm (consult OCC documentation).

  • smoothing (Optional[Tuple[float, float, float]]) – optional tuple of 3 weights use for variational smoothing (default: None)

  • minDeg (int) – minimum spline degree. Enforced only when smothing is None (default: 1)

  • maxDeg (int) – maximum spline degree (default: 6)

Return type

Face

normalAt(locationVector: Optional[Vector] = None) → Vector[source]

Computes the normal vector at the desired location on the face.

Returns

a vector representing the direction

Parameters

locationVector (a vector that lies on the surface.) – the location to compute the normal at. If none, the center of the face is used.

Return type

Vector

thicken(thickness: float) → Solid[source]

Return a thickened face

Parameters

thickness (float) –

Return type

Solid

toArcs(tolerance: float = 0.001) → Face[source]

Approximate planar face with arcs and straight line segments.

Parameters

tolerance (float) – Approximation tolerance.

Return type

Face

toPln() → gp_Pln[source]

Convert this face to a gp_Pln.

Note the Location of the resulting plane may not equal the center of this face, however the resulting plane will still contain the center of this face.

Return type

gp_Pln

class cadquery.Location(t: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]])[source]

Bases: object

Location in 3D space. Depending on usage can be absolute or relative.

This class wraps the TopLoc_Location class from OCCT. It can be used to move Shape objects in both relative and absolute manner. It is the preferred type to locate objects in CQ.

Parameters

t (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

__init__(t: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], ax: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], angle: Union[int, float]) → None[source]
__init__(T: TopLoc_Location) → None
__init__(t: Plane) → None
__init__(x: Union[int, float] = 0, y: Union[int, float] = 0, z: Union[int, float] = 0, rx: Union[int, float] = 0, ry: Union[int, float] = 0, rz: Union[int, float] = 0) → None
__init__(t: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], angles: Tuple[Union[int, float], Union[int, float], Union[int, float]]) → None
__init__(t: Plane, v: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → None
__init__(T: gp_Trsf) → None
__init__(t: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → None

Location with translation t with respect to the original location.

Location with translation (x,y,z) and 3 rotation angles.

Location corresponding to the location of the Plane t.

Location corresponding to the angular location of the Plane t with translation v.

Location wrapping the low-level TopLoc_Location object t

Location wrapping the low-level gp_Trsf object t

Location with translation t and rotation around ax by angle

with respect to the original location.

Location with translation t and 3 rotation angles.

Parameters

t (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

Return type

None

__weakref__

list of weak references to the object (if defined)

toTuple() → Tuple[Tuple[float, float, float], Tuple[float, float, float]][source]

Convert the location to a translation, rotation tuple.

Return type

Tuple[Tuple[float, float, float], Tuple[float, float, float]]

class cadquery.Matrix[source]
class cadquery.Matrix(matrix: Union[gp_GTrsf, gp_Trsf])
class cadquery.Matrix(matrix: Sequence[Sequence[float]])

Bases: object

A 3d , 4x4 transformation matrix.

Used to move geometry in space.

The provided “matrix” parameter may be None, a gp_GTrsf, or a nested list of values.

If given a nested list, it is expected to be of the form:

[[m11, m12, m13, m14],

[m21, m22, m23, m24], [m31, m32, m33, m34]]

A fourth row may be given, but it is expected to be: [0.0, 0.0, 0.0, 1.0] since this is a transform matrix.

__getitem__(rc: Tuple[int, int]) → float[source]

Provide Matrix[r, c] syntax for accessing individual values. The row and column parameters start at zero, which is consistent with most python libraries, but is counter to gp_GTrsf(), which is 1-indexed.

Parameters

rc (Tuple[int, int]) –

Return type

float

__init__() → None[source]
__init__(matrix: Union[gp_GTrsf, gp_Trsf]) → None
__init__(matrix: Sequence[Sequence[float]]) → None
__repr__() → str[source]

Generate a valid python expression representing this Matrix

Return type

str

__weakref__

list of weak references to the object (if defined)

transposed_list() → Sequence[float][source]

Needed by the cqparts gltf exporter

Return type

Sequence[float]

class cadquery.NearestToPointSelector(pnt)[source]

Bases: Selector

Selects object nearest the provided point.

If the object is a vertex or point, the distance is used. For other kinds of shapes, the center of mass is used to to compute which is closest.

Applicability: All Types of Shapes

Example:

CQ(aCube).vertices(NearestToPointSelector((0, 1, 0)))

returns the vertex of the unit cube closest to the point x=0,y=1,z=0

__init__(pnt)[source]
filter(objectList: Sequence[Shape])[source]

Filter the provided list.

The default implementation returns the original list unfiltered.

Parameters

objectList (list of OCCT primitives) – list to filter

Returns

filtered list

class cadquery.ParallelDirSelector(vector: Vector, tolerance: float = 0.0001)[source]

Bases: BaseDirSelector

Selects objects parallel with the provided direction.

Applicability:

Linear Edges Planar Faces

Use the string syntax shortcut |(X|Y|Z) if you want to select based on a cardinal direction.

Example:

CQ(aCube).faces(ParallelDirSelector((0, 0, 1)))

selects faces with the normal parallel to the z direction, and is equivalent to:

CQ(aCube).faces("|Z")
Parameters

  • vector (Vector) –

  • tolerance (float) –

test(vec: Vector) → bool[source]

Test a specified vector. Subclasses override to provide other implementations

Parameters

vec (Vector) –

Return type

bool

class cadquery.PerpendicularDirSelector(vector: Vector, tolerance: float = 0.0001)[source]

Bases: BaseDirSelector

Selects objects perpendicular with the provided direction.

Applicability:

Linear Edges Planar Faces

Use the string syntax shortcut #(X|Y|Z) if you want to select based on a cardinal direction.

Example:

CQ(aCube).faces(PerpendicularDirSelector((0, 0, 1)))

selects faces with the normal perpendicular to the z direction, and is equivalent to:

CQ(aCube).faces("#Z")
Parameters

  • vector (Vector) –

  • tolerance (float) –

test(vec: Vector) → bool[source]

Test a specified vector. Subclasses override to provide other implementations

Parameters

vec (Vector) –

Return type

bool

class cadquery.Plane(origin: Union[Tuple[float, float, float], Vector], xDir: Optional[Union[Tuple[float, float, float], Vector]] = None, normal: Union[Tuple[float, float, float], Vector] = (0, 0, 1))[source]

Bases: object

A 2D coordinate system in space

A 2D coordinate system in space, with the x-y axes on the plane, and a particular point as the origin.

A plane allows the use of 2D coordinates, which are later converted to global, 3d coordinates when the operations are complete.

Frequently, it is not necessary to create work planes, as they can be created automatically from faces.

Parameters

  • origin (Union[Tuple[float, float, float], Vector]) –

  • xDir (Vector) –

  • normal (Union[Tuple[float, float, float], Vector]) –

__eq__(other)[source]

Return self==value.

__hash__ = None
__init__(origin: Union[Tuple[float, float, float], Vector], xDir: Optional[Union[Tuple[float, float, float], Vector]] = None, normal: Union[Tuple[float, float, float], Vector] = (0, 0, 1))[source]

Create a Plane with an arbitrary orientation

Parameters

  • origin (Union[Tuple[float, float, float], Vector]) – the origin in global coordinates

  • xDir (Optional[Union[Tuple[float, float, float], Vector]]) – an optional vector representing the xDirection.

  • normal (Union[Tuple[float, float, float], Vector]) – the normal direction for the plane

Raises

ValueError – if the specified xDir is not orthogonal to the provided normal

__ne__(other)[source]

Return self!=value.

__repr__()[source]

Return repr(self).

__weakref__

list of weak references to the object (if defined)

classmethod named(stdName: str, origin=(0, 0, 0)) → Plane[source]

Create a predefined Plane based on the conventional names.

Parameters

  • stdName (string) – one of (XY|YZ|ZX|XZ|YX|ZY|front|back|left|right|top|bottom)

  • origin (3-tuple of the origin of the new plane, in global coordinates.) – the desired origin, specified in global coordinates

Return type

Plane

Available named planes are as follows. Direction references refer to the global directions.

Name

xDir

yDir

zDir

XY

+x

+y

+z

YZ

+y

+z

+x

ZX

+z

+x

+y

XZ

+x

+z

-y

YX

+y

+x

-z

ZY

+z

+y

-x

front

+x

+y

+z

back

-x

+y

-z

left

+z

+y

-x

right

-z

+y

+x

top

+x

-z

+y

bottom

+x

+z

-y
rotated(rotate=(0, 0, 0))[source]

Returns a copy of this plane, rotated about the specified axes

Since the z axis is always normal the plane, rotating around Z will always produce a plane that is parallel to this one.

The origin of the workplane is unaffected by the rotation.

Rotations are done in order x, y, z. If you need a different order, manually chain together multiple rotate() commands.

Parameters

rotate – Vector [xDegrees, yDegrees, zDegrees]

Returns

a copy of this plane rotated as requested.

setOrigin2d(x, y)[source]

Set a new origin in the plane itself

Set a new origin in the plane itself. The plane’s orientation and xDrection are unaffected.

Parameters

  • x (float) – offset in the x direction

  • y (float) – offset in the y direction

Returns

void

The new coordinates are specified in terms of the current 2D system. As an example:

p = Plane.XY() p.setOrigin2d(2, 2) p.setOrigin2d(2, 2)

results in a plane with its origin at (x, y) = (4, 4) in global coordinates. Both operations were relative to local coordinates of the plane.

toLocalCoords(obj)[source]

Project the provided coordinates onto this plane

Parameters

obj – an object or vector to convert

Returns

an object of the same type, but converted to local coordinates

Most of the time, the z-coordinate returned will be zero, because most operations based on a plane are all 2D. Occasionally, though, 3D points outside of the current plane are transformed. One such example is Workplane.box(), where 3D corners of a box are transformed to orient the box in space correctly.

toWorldCoords(tuplePoint) → Vector[source]

Convert a point in local coordinates to global coordinates

Parameters

tuplePoint (a 2 or three tuple of float. The third value is taken to be zero if not supplied.) – point in local coordinates to convert.

Returns

a Vector in global coordinates

Return type

Vector

class cadquery.Selector[source]

Bases: object

Filters a list of objects.

Filters must provide a single method that filters objects.

__weakref__

list of weak references to the object (if defined)

filter(objectList: Sequence[Shape]) → List[Shape][source]

Filter the provided list.

The default implementation returns the original list unfiltered.

Parameters

objectList (list of OCCT primitives) – list to filter

Returns

filtered list

Return type

List[Shape]

class cadquery.Shape(obj: TopoDS_Shape)[source]

Bases: object

Represents a shape in the system. Wraps TopoDS_Shape.

Parameters

obj (TopoDS_Shape) –

Area() → float[source]
Returns

The surface area of all faces in this Shape

Return type

float

BoundingBox(tolerance: Optional[float] = None) → BoundBox[source]

Create a bounding box for this Shape.

Parameters

tolerance (Optional[float]) – Tolerance value passed to BoundBox

Returns

A BoundBox object for this Shape

Return type

BoundBox

Center() → Vector[source]
Returns

The point of the center of mass of this Shape

Return type

Vector

CenterOfBoundBox(tolerance: Optional[float] = None) → Vector[source]
Parameters

tolerance (Optional[float]) – Tolerance passed to the BoundingBox() method

Returns

Center of the bounding box of this shape

Return type

Vector

Closed() → bool[source]
Returns

The closedness flag

Return type

bool

static CombinedCenter(objects: Iterable[Shape]) → Vector[source]

Calculates the center of mass of multiple objects.

Parameters

objects (Iterable[Shape]) – A list of objects with mass

Return type

Vector

static CombinedCenterOfBoundBox(objects: List[Shape]) → Vector[source]

Calculates the center of a bounding box of multiple objects.

Parameters

objects (List[Shape]) – A list of objects

Return type

Vector

CompSolids() → List[CompSolid][source]
Returns

All the compsolids in this Shape

Return type

List[CompSolid]

Compounds() → List[Compound][source]
Returns

All the compounds in this Shape

Return type

List[Compound]

Edges() → List[Edge][source]
Returns

All the edges in this Shape

Return type

List[Edge]

Faces() → List[Face][source]
Returns

All the faces in this Shape

Return type

List[Face]

Shells() → List[Shell][source]
Returns

All the shells in this Shape

Return type

List[Shell]

Solids() → List[Solid][source]
Returns

All the solids in this Shape

Return type

List[Solid]

Vertices() → List[Vertex][source]
Returns

All the vertices in this Shape

Return type

List[Vertex]

Volume() → float[source]
Returns

The volume of this Shape

Return type

float

Wires() → List[Wire][source]
Returns

All the wires in this Shape

Return type

List[Wire]

__add__(other: Shape) → Shape[source]

Fuse self and other.

Parameters

other (Shape) –

Return type

Shape

__eq__(other) → bool[source]

Return self==value.

Return type

bool

__hash__() → int[source]

Return hash(self).

Return type

int

__init__(obj: TopoDS_Shape)[source]
Parameters

obj (TopoDS_Shape) –

__iter__() → Iterator[Shape][source]

Iterate over subshapes.

Return type

Iterator[Shape]

__mul__(other: Shape) → Shape[source]

Intersect self and other.

Parameters

other (Shape) –

Return type

Shape

__sub__(other: Shape) → Shape[source]

Subtract other from self.

Parameters

other (Shape) –

Return type

Shape

__truediv__(other: Shape) → Shape[source]

Split self with other.

Parameters

other (Shape) –

Return type

Shape

__weakref__

list of weak references to the object (if defined)

ancestors(shape: Shape, kind: Literal['Vertex', 'Edge', 'Wire', 'Face', 'Shell', 'Solid', 'CompSolid', 'Compound']) → Compound[source]

Iterate over ancestors, i.e. shapes of same kind within shape that contain self.

Parameters

  • shape (Shape) –

  • kind (Literal['Vertex', 'Edge', 'Wire', 'Face', 'Shell', 'Solid', 'CompSolid', 'Compound']) –

Return type

Compound

classmethod cast(obj: TopoDS_Shape, forConstruction: bool = False) → Shape[source]

Returns the right type of wrapper, given a OCCT object

Parameters

  • obj (TopoDS_Shape) –

  • forConstruction (bool) –

Return type

Shape

static centerOfMass(obj: Shape) → Vector[source]

Calculates the center of ‘mass’ of an object.

Parameters

obj (Shape) – Compute the center of mass of this object

Return type

Vector

clean() → T[source]

Experimental clean using ShapeUpgrade

Parameters

self (T) –

Return type

T

static computeMass(obj: Shape) → float[source]

Calculates the ‘mass’ of an object.

Parameters

obj (Shape) – Compute the mass of this object

Return type

float

copy(mesh: bool = False) → T[source]

Creates a new object that is a copy of this object.

Parameters

  • self (T) –

  • mesh (bool) – should I copy the triangulation too (default: False)

Returns

a copy of the object

Return type

T

cut(*toCut: Shape, tol: Optional[float] = None) → Shape[source]

Remove the positional arguments from this Shape.

Parameters

  • tol (Optional[float]) – Fuzzy mode tolerance

  • toCut (Shape) –

Return type

Shape

distance(other: Shape) → float[source]

Minimal distance between two shapes

Parameters

other (Shape) –

Return type

float

distances(*others: Shape) → Iterator[float][source]

Minimal distances to between self and other shapes

Parameters

others (Shape) –

Return type

Iterator[float]

edges(selector: Optional[Union[Selector, str]] = None) → Shape[source]

Select edges.

Parameters

selector (Optional[Union[Selector, str]]) –

Return type

Shape

export(fname: str, tolerance: float = 0.1, angularTolerance: float = 0.1, opt: Optional[Dict[str, Any]] = None)[source]

Export Shape to file.

Parameters

  • self (T) –

  • fname (str) –

  • tolerance (float) –

  • angularTolerance (float) –

  • opt (Optional[Dict[str, Any]]) –

exportBrep(f: Union[str, BytesIO]) → bool[source]

Export this shape to a BREP file

Parameters

f (Union[str, BytesIO]) –

Return type

bool

exportStep(fileName: str, **kwargs) → IFSelect_ReturnStatus[source]

Export this shape to a STEP file.

kwargs is used to provide optional keyword arguments to configure the exporter.

Parameters

  • fileName (str) – Path and filename for writing.

  • write_pcurves (bool) –

    Enable or disable writing parametric curves to the STEP file. Default True.

    If False, writes STEP file without pcurves. This decreases the size of the resulting STEP file.

  • precision_mode (int) – Controls the uncertainty value for STEP entities. Specify -1, 0, or 1. Default 0. See OCCT documentation.

Return type

IFSelect_ReturnStatus

exportStl(fileName: str, tolerance: float = 0.001, angularTolerance: float = 0.1, ascii: bool = False, relative: bool = True, parallel: bool = True) → bool[source]

Exports a shape to a specified STL file.

Parameters

  • fileName (str) – The path and file name to write the STL output to.

  • tolerance (float) – A linear deflection setting which limits the distance between a curve and its tessellation. Setting this value too low will result in large meshes that can consume computing resources. Setting the value too high can result in meshes with a level of detail that is too low. Default is 1e-3, which is a good starting point for a range of cases.

  • angularTolerance (float) – Angular deflection setting which limits the angle between subsequent segments in a polyline. Default is 0.1.

  • ascii (bool) – Export the file as ASCII (True) or binary (False) STL format. Default is binary.

  • relative (bool) – If True, tolerance will be scaled by the size of the edge being meshed. Default is True. Setting this value to True may cause large features to become faceted, or small features dense.

  • parallel (bool) – If True, OCCT will use parallel processing to mesh the shape. Default is True.

Return type

bool

faces(selector: Optional[Union[Selector, str]] = None) → Shape[source]

Select faces.

Parameters

selector (Optional[Union[Selector, str]]) –

Return type

Shape

facesIntersectedByLine(point: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], axis: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], tol: float = 0.0001, direction: Optional[Literal['AlongAxis', 'Opposite']] = None)[source]

Computes the intersections between the provided line and the faces of this Shape

Parameters

  • point (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – Base point for defining a line

  • axis (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – Axis on which the line rests

  • tol (float) – Intersection tolerance

  • direction (Optional[Literal['AlongAxis', 'Opposite']]) – Valid values: “AlongAxis”, “Opposite”; If specified, will ignore all faces that are not in the specified direction including the face where the point lies if it is the case

Returns

A list of intersected faces sorted by distance from point

fix() → T[source]

Try to fix shape if not valid

Parameters

self (T) –

Return type

T

fuse(*toFuse: Shape, glue: bool = False, tol: Optional[float] = None) → Shape[source]

Fuse the positional arguments with this Shape.

Parameters

  • glue (bool) – Sets the glue option for the algorithm, which allows increasing performance of the intersection of the input shapes

  • tol (Optional[float]) – Fuzzy mode tolerance

  • toFuse (Shape) –

Return type

Shape

geomType() → Literal['Vertex', 'Wire', 'Shell', 'Solid', 'Compound', 'PLANE', 'CYLINDER', 'CONE', 'SPHERE', 'TORUS', 'BEZIER', 'BSPLINE', 'REVOLUTION', 'EXTRUSION', 'OFFSET', 'OTHER', 'LINE', 'CIRCLE', 'ELLIPSE', 'HYPERBOLA', 'PARABOLA'][source]

Gets the underlying geometry type.

Implementations can return any values desired, but the values the user uses in type filters should correspond to these.

As an example, if a user does:

CQ(object).faces("%mytype")

The expectation is that the geomType attribute will return ‘mytype’

The return values depend on the type of the shape:

Vertex: always ‘Vertex’
Edge: LINE, CIRCLE, ELLIPSE, HYPERBOLA, PARABOLA, BEZIER,
BSPLINE, OFFSET, OTHER
Face: PLANE, CYLINDER, CONE, SPHERE, TORUS, BEZIER, BSPLINE,
REVOLUTION, EXTRUSION, OFFSET, OTHER
Solid: ‘Solid’
Shell: ‘Shell’
Compound: ‘Compound’
Wire: ‘Wire’
Returns

A string according to the geometry type

Return type

Literal[‘Vertex’, ‘Wire’, ‘Shell’, ‘Solid’, ‘Compound’, ‘PLANE’, ‘CYLINDER’, ‘CONE’, ‘SPHERE’, ‘TORUS’, ‘BEZIER’, ‘BSPLINE’, ‘REVOLUTION’, ‘EXTRUSION’, ‘OFFSET’, ‘OTHER’, ‘LINE’, ‘CIRCLE’, ‘ELLIPSE’, ‘HYPERBOLA’, ‘PARABOLA’]

hashCode() → int[source]

Returns a hashed value denoting this shape. It is computed from the TShape and the Location. The Orientation is not used.

Return type

int

classmethod importBrep(f: Union[str, BytesIO]) → Shape[source]

Import shape from a BREP file

Parameters

f (Union[str, BytesIO]) –

Return type

Shape

intersect(*toIntersect: Shape, tol: Optional[float] = None) → Shape[source]

Intersection of the positional arguments and this Shape.

Parameters

  • tol (Optional[float]) – Fuzzy mode tolerance

  • toIntersect (Shape) –

Return type

Shape

isEqual(other: Shape) → bool[source]

Returns True if two shapes are equal, i.e. if they share the same TShape with the same Locations and Orientations. Also see isSame().

Parameters

other (Shape) –

Return type

bool

isNull() → bool[source]

Returns true if this shape is null. In other words, it references no underlying shape with the potential to be given a location and an orientation.

Return type

bool

isSame(other: Shape) → bool[source]

Returns True if other and this shape are same, i.e. if they share the same TShape with the same Locations. Orientations may differ. Also see isEqual()

Parameters

other (Shape) –

Return type

bool

isValid() → bool[source]

Returns True if no defect is detected on the shape S or any of its subshapes. See the OCCT docs on BRepCheck_Analyzer::IsValid for a full description of what is checked.

Return type

bool

locate(loc: Location) → T[source]

Apply a location in absolute sense to self

Parameters
Return type

T

located(loc: Location) → T[source]

Apply a location in absolute sense to a copy of self

Parameters
Return type

T

location() → Location[source]

Return the current location

Return type

Location

static matrixOfInertia(obj: Shape) → List[List[float]][source]

Calculates the matrix of inertia of an object. Since the part’s density is unknown, this result is inertia/density with units of [1/length]. :param obj: Compute the matrix of inertia of this object

Parameters

obj (Shape) –

Return type

List[List[float]]

mesh(tolerance: float, angularTolerance: float = 0.1)[source]

Generate triangulation if none exists.

Parameters

  • tolerance (float) –

  • angularTolerance (float) –

mirror(mirrorPlane: Union[Literal['XY', 'YX', 'XZ', 'ZX', 'YZ', 'ZY'], Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]] = 'XY', basePointVector: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]] = (0, 0, 0)) → Shape[source]

Applies a mirror transform to this Shape. Does not duplicate objects about the plane.

Parameters

  • mirrorPlane (Union[Literal['XY', 'YX', 'XZ', 'ZX', 'YZ', 'ZY'], Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – The direction of the plane to mirror about - one of ‘XY’, ‘XZ’ or ‘YZ’

  • basePointVector (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – The origin of the plane to mirror about

Returns

The mirrored shape

Return type

Shape

move(loc: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → T[source]
move(loc: Location) → T
move(x: Union[float, int] = 0, y: Union[float, int] = 0, z: Union[float, int] = 0, rx: Union[float, int] = 0, ry: Union[float, int] = 0, rz: Union[float, int] = 0) → T

Apply a location in relative sense (i.e. update current location) to self

Parameters
Return type

T

moved(x: Union[float, int] = 0, y: Union[float, int] = 0, z: Union[float, int] = 0, rx: Union[float, int] = 0, ry: Union[float, int] = 0, rz: Union[float, int] = 0) → T[source]
moved(loc: Sequence[Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]]) → T
moved(loc: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → T
moved(loc1: Location, loc2: Location, *locs: Location) → T
moved(loc1: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], loc2: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], *locs: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → T
moved(locs: Sequence[Location]) → T
moved(loc: Location) → T

Apply a location in relative sense (i.e. update current location) to a copy of self

Parameters
Return type

T

rotate(startVector: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], endVector: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], angleDegrees: float) → T[source]

Rotates a shape around an axis.

Parameters

  • self (T) –

  • startVector (either a 3-tuple or a Vector) – start point of rotation axis

  • endVector (either a 3-tuple or a Vector) – end point of rotation axis

  • angleDegrees (float) – angle to rotate, in degrees

Returns

a copy of the shape, rotated

Return type

T

scale(factor: float) → Shape[source]

Scales this shape through a transformation.

Parameters

factor (float) –

Return type

Shape

shells(selector: Optional[Union[Selector, str]] = None) → Shape[source]

Select shells.

Parameters

selector (Optional[Union[Selector, str]]) –

Return type

Shape

siblings(shape: Shape, kind: Literal['Vertex', 'Edge', 'Wire', 'Face', 'Shell', 'Solid', 'CompSolid', 'Compound'], level: int = 1) → Compound[source]

Iterate over siblings, i.e. shapes within shape that share subshapes of kind with self.

Parameters

  • shape (Shape) –

  • kind (Literal['Vertex', 'Edge', 'Wire', 'Face', 'Shell', 'Solid', 'CompSolid', 'Compound']) –

  • level (int) –

Return type

Compound

solids(selector: Optional[Union[Selector, str]] = None) → Shape[source]

Select solids.

Parameters

selector (Optional[Union[Selector, str]]) –

Return type

Shape

split(*splitters: Shape) → Shape[source]

Split this shape with the positional arguments.

Parameters

splitters (Shape) –

Return type

Shape

toSplines(degree: int = 3, tolerance: float = 0.001, nurbs: bool = False) → T[source]

Approximate shape with b-splines of the specified degree.

Parameters

  • self (T) –

  • degree (int) – Maximum degree.

  • tolerance (float) – Approximation tolerance.

  • nurbs (bool) – Use rational splines.

Return type

T

toVtkPolyData(tolerance: Optional[float] = None, angularTolerance: Optional[float] = None, normals: bool = False) → vtkPolyData[source]

Convert shape to vtkPolyData

Parameters

  • tolerance (Optional[float]) –

  • angularTolerance (Optional[float]) –

  • normals (bool) –

Return type

vtkPolyData

transformGeometry(tMatrix: Matrix) → Shape[source]

Transforms this shape by tMatrix.

WARNING: transformGeometry will sometimes convert lines and circles to splines, but it also has the ability to handle skew and stretching transformations.

If your transformation is only translation and rotation, it is safer to use transformShape(), which doesn’t change the underlying type of the geometry, but cannot handle skew transformations.

Parameters

tMatrix (Matrix) – The transformation matrix

Returns

a copy of the object, but with geometry transformed instead of just rotated.

Return type

Shape

transformShape(tMatrix: Matrix) → Shape[source]

Transforms this Shape by tMatrix. Also see transformGeometry().

Parameters

tMatrix (Matrix) – The transformation matrix

Returns

a copy of the object, transformed by the provided matrix, with all objects keeping their type

Return type

Shape

translate(vector: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → T[source]

Translates this shape through a transformation.

Parameters

  • self (T) –

  • vector (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

Return type

T

vertices(selector: Optional[Union[Selector, str]] = None) → Shape[source]

Select vertices.

Parameters

selector (Optional[Union[Selector, str]]) –

Return type

Shape

wires(selector: Optional[Union[Selector, str]] = None) → Shape[source]

Select wires.

Parameters

selector (Optional[Union[Selector, str]]) –

Return type

Shape

class cadquery.Shell(obj: TopoDS_Shape)[source]

Bases: Shape

the outer boundary of a surface

Parameters

obj (TopoDS_Shape) –

classmethod makeShell(listOfFaces: Iterable[Face]) → Shell[source]

Makes a shell from faces.

Parameters

listOfFaces (Iterable[Face]) –

Return type

Shell

class cadquery.Sketch(parent: ~typing.Any = None, locs: ~typing.Iterable[~cadquery.occ_impl.geom.Location] = (<cadquery.occ_impl.geom.Location object>, ), obj: ~typing.Optional[~cadquery.occ_impl.shapes.Compound] = None)[source]

Bases: object

2D sketch. Supports faces, edges and edges with constraints based construction.

Parameters
__add__(other: Sketch) → T[source]

Fuse self and other.

Parameters

  • self (T) –

  • other (Sketch) –

Return type

T

__init__(parent: ~typing.Any = None, locs: ~typing.Iterable[~cadquery.occ_impl.geom.Location] = (<cadquery.occ_impl.geom.Location object>, ), obj: ~typing.Optional[~cadquery.occ_impl.shapes.Compound] = None)[source]

Construct an empty sketch.

Parameters

  • self (T) –

  • parent (Any) –

  • locs (Iterable[Location]) –

  • obj (Optional[Compound]) –

__iter__() → Iterator[Face][source]

Iterate over faces-locations combinations. If not faces are present iterate over edges:

Return type

Iterator[Face]

__mul__(other: Sketch) → T[source]

Intersect self and other.

Parameters

  • self (T) –

  • other (Sketch) –

Return type

T

__sub__(other: Sketch) → T[source]

Subtract other from self.

Parameters

  • self (T) –

  • other (Sketch) –

Return type

T

__truediv__(other: Sketch) → T[source]

Split self with other.

Parameters

  • self (T) –

  • other (Sketch) –

Return type

T

__weakref__

list of weak references to the object (if defined)

add() → T[source]

Add selection to the underlying faces.

Parameters

self (T) –

Return type

T

apply(f: Callable[[Iterable[Union[Shape, Location]]], Iterable[Union[Shape, Location]]])[source]

Apply a callable to all items at once.

Parameters
Returns

Sketch object with f applied to all items.

arc(p1: Union[Vector, Tuple[Union[int, float], Union[int, float]]], p2: Union[Vector, Tuple[Union[int, float], Union[int, float]]], p3: Union[Vector, Tuple[Union[int, float], Union[int, float]]], tag: Optional[str] = None, forConstruction: bool = False) → T[source]
arc(c: Union[Vector, Tuple[Union[int, float], Union[int, float]]], r: Union[int, float], a: Union[int, float], da: Union[int, float], tag: Optional[str] = None, forConstruction: bool = False) → T
arc(p2: Union[Vector, Tuple[Union[int, float], Union[int, float]]], p3: Union[Vector, Tuple[Union[int, float], Union[int, float]]], tag: Optional[str] = None, forConstruction: bool = False) → T

Construct an arc.

Parameters

  • self (T) –

  • p1 (Union[Vector, Tuple[Union[int, float], Union[int, float]]]) –

  • p2 (Union[Vector, Tuple[Union[int, float], Union[int, float]]]) –

  • p3 (Union[Vector, Tuple[Union[int, float], Union[int, float]]]) –

  • tag (Optional[str]) –

  • forConstruction (bool) –

Return type

T

assemble(mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None) → T[source]

Assemble edges into faces.

Parameters

  • self (T) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

Return type

T

bezier(pts: Iterable[Union[Vector, Tuple[Union[int, float], Union[int, float]]]], tag: Optional[str] = None, forConstruction: bool = False) → T[source]

Construct an bezier curve.

The edge will pass through the last points, and the inner points are bezier control points.

Parameters

  • self (T) –

  • pts (Iterable[Union[Vector, Tuple[Union[int, float], Union[int, float]]]]) –

  • tag (Optional[str]) –

  • forConstruction (bool) –

Return type

T

chamfer(d: Union[int, float]) → T[source]

Add a chamfer based on current selection.

Parameters

  • self (T) –

  • d (Union[int, float]) –

Return type

T

circle(r: Union[int, float], mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None) → T[source]

Construct a circular face.

Parameters

  • self (T) –

  • r (Union[int, float]) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

Return type

T

clean() → T[source]

Remove internal wires.

Parameters

self (T) –

Return type

T

close(tag: Optional[str] = None) → T[source]

Connect last edge to the first one.

Parameters

  • self (T) –

  • tag (Optional[str]) –

Return type

T

constrain(tag: str, constraint: Literal['Fixed', 'FixedPoint', 'Coincident', 'Angle', 'Length', 'Distance', 'Radius', 'Orientation', 'ArcAngle'], arg: Any) → T[source]
constrain(tag1: str, tag2: str, constraint: Literal['Fixed', 'FixedPoint', 'Coincident', 'Angle', 'Length', 'Distance', 'Radius', 'Orientation', 'ArcAngle'], arg: Any) → T

Add a constraint.

Parameters

  • self (T) –

  • tag (str) –

  • constraint (Literal['Fixed', 'FixedPoint', 'Coincident', 'Angle', 'Length', 'Distance', 'Radius', 'Orientation', 'ArcAngle']) –

  • arg (Any) –

Return type

T

copy() → T[source]

Create a partial copy of the sketch.

Parameters

self (T) –

Return type

T

delete() → T[source]

Delete selected object.

Parameters

self (T) –

Return type

T

distribute(n: int, start: Union[int, float] = 0, stop: Union[int, float] = 1, rotate: bool = True) → T[source]

Distribute locations along selected edges or wires.

Parameters

  • self (T) –

  • n (int) –

  • start (Union[int, float]) –

  • stop (Union[int, float]) –

  • rotate (bool) –

Return type

T

each(callback: Callable[[Location], Union[Face, Sketch, Compound]], mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None, ignore_selection: bool = False) → T[source]

Apply a callback on all applicable entities.

Parameters

  • self (T) –

  • callback (Callable[[Location], Union[Face, Sketch, Compound]]) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

  • ignore_selection (bool) –

Return type

T

edge(val: Edge, tag: Optional[str] = None, forConstruction: bool = False) → T[source]

Add an edge to the sketch.

Parameters

  • self (T) –

  • val (Edge) –

  • tag (Optional[str]) –

  • forConstruction (bool) –

Return type

T

edges(s: Optional[Union[str, Selector]] = None, tag: Optional[str] = None) → T[source]

Select edges.

Parameters

  • self (T) –

  • s (Optional[Union[str, Selector]]) –

  • tag (Optional[str]) –

Return type

T

ellipse(a1: Union[int, float], a2: Union[int, float], angle: Union[int, float] = 0, mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None) → T[source]

Construct an elliptical face.

Parameters

  • self (T) –

  • a1 (Union[int, float]) –

  • a2 (Union[int, float]) –

  • angle (Union[int, float]) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

Return type

T

export(fname: str, tolerance: float = 0.1, angularTolerance: float = 0.1, opt: Optional[Dict[str, Any]] = None) → T[source]

Export Sketch to file.

Parameters

  • self (T) –

  • path – Filename.

  • tolerance (float) – the deflection tolerance, in model units. Default 0.1.

  • angularTolerance (float) – the angular tolerance, in radians. Default 0.1.

  • opt (Optional[Dict[str, Any]]) – additional options passed to the specific exporter. Default None.

  • fname (str) –

Returns

Self.

Return type

T

face(b: Union[Wire, Iterable[Edge], Shape, T], angle: Union[int, float] = 0, mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None, ignore_selection: bool = False) → T[source]

Construct a face from a wire or edges.

Parameters

  • self (T) –

  • b (Union[Wire, Iterable[Edge], Shape, T]) –

  • angle (Union[int, float]) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

  • ignore_selection (bool) –

Return type

T

faces(s: Optional[Union[str, Selector]] = None, tag: Optional[str] = None) → T[source]

Select faces.

Parameters

  • self (T) –

  • s (Optional[Union[str, Selector]]) –

  • tag (Optional[str]) –

Return type

T

fillet(d: Union[int, float]) → T[source]

Add a fillet based on current selection.

Parameters

  • self (T) –

  • d (Union[int, float]) –

Return type

T

filter(f: Callable[[Union[Shape, Location]], bool]) → T[source]

Filter items using a boolean predicate.

Parameters

  • self (T) –

  • f (Callable[[Union[Shape, Location]], bool]) – Callable to be used for filtering.

Returns

Sketch object with filtered items.

Return type

T

finalize() → Any[source]

Finish sketch construction and return the parent.

Return type

Any

hull(mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None) → T[source]

Generate a convex hull from current selection or all objects.

Parameters

  • self (T) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

Return type

T

importDXF(filename: str, tol: float = 1e-06, exclude: List[str] = [], include: List[str] = [], angle: Union[int, float] = 0, mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None) → T[source]

Import a DXF file and construct face(s)

Parameters

  • self (T) –

  • filename (str) –

  • tol (float) –

  • exclude (List[str]) –

  • include (List[str]) –

  • angle (Union[int, float]) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

Return type

T

invoke(f: Union[Callable[[T], T], Callable[[T], None], Callable[[], None]])[source]

Invoke a callable mapping Sketch to Sketch or None. Supports also callables that take no arguments such as breakpoint. Returns self if callable returns None.

Parameters

  • self (T) –

  • f (Union[Callable[[T], T], Callable[[T], None], Callable[[], None]]) – Callable to be invoked.

Returns

Sketch object.

located(loc: Location) → T[source]

Create a partial copy of the sketch with a new location.

Parameters
Return type

T

map(f: Callable[[Union[Shape, Location]], Union[Shape, Location]])[source]

Apply a callable to every item separately.

Parameters

  • self (T) –

  • f (Callable[[Union[Shape, Location]], Union[Shape, Location]]) – Callable to be applied to every item separately.

Returns

Sketch object with f applied to all items.

moved(loc: Location) → T[source]
moved(loc1: Location, loc2: Location, *locs: Location) → T
moved(locs: Sequence[Location]) → T
moved(x: Union[int, float] = 0, y: Union[int, float] = 0, z: Union[int, float] = 0, rx: Union[int, float] = 0, ry: Union[int, float] = 0, rz: Union[int, float] = 0) → T
moved(loc: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → T
moved(loc1: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], loc2: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], *locs: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → T
moved(loc: Sequence[Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]]) → T

Create a partial copy of the sketch with moved _faces.

offset(d: Union[int, float], mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None) → T[source]

Offset selected wires or edges.

Parameters

  • self (T) –

  • d (Union[int, float]) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

Return type

T

parray(r: Union[int, float], a1: Union[int, float], da: Union[int, float], n: int, rotate: bool = True) → T[source]

Generate a polar array of locations.

Parameters

  • self (T) –

  • r (Union[int, float]) –

  • a1 (Union[int, float]) –

  • da (Union[int, float]) –

  • n (int) –

  • rotate (bool) –

Return type

T

polygon(pts: Iterable[Union[Vector, Tuple[Union[int, float], Union[int, float]]]], angle: Union[int, float] = 0, mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None) → T[source]

Construct a polygonal face.

Parameters

  • self (T) –

  • pts (Iterable[Union[Vector, Tuple[Union[int, float], Union[int, float]]]]) –

  • angle (Union[int, float]) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

Return type

T

push(locs: Iterable[Union[Location, Vector, Tuple[Union[int, float], Union[int, float]]]], tag: Optional[str] = None) → T[source]

Set current selection to given locations or points.

Parameters

  • self (T) –

  • locs (Iterable[Union[Location, Vector, Tuple[Union[int, float], Union[int, float]]]]) –

  • tag (Optional[str]) –

Return type

T

rarray(xs: Union[int, float], ys: Union[int, float], nx: int, ny: int) → T[source]

Generate a rectangular array of locations.

Parameters

  • self (T) –

  • xs (Union[int, float]) –

  • ys (Union[int, float]) –

  • nx (int) –

  • ny (int) –

Return type

T

rect(w: Union[int, float], h: Union[int, float], angle: Union[int, float] = 0, mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None) → T[source]

Construct a rectangular face.

Parameters

  • self (T) –

  • w (Union[int, float]) –

  • h (Union[int, float]) –

  • angle (Union[int, float]) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

Return type

T

regularPolygon(r: Union[int, float], n: int, angle: Union[int, float] = 0, mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None) → T[source]

Construct a regular polygonal face.

Parameters

  • self (T) –

  • r (Union[int, float]) –

  • n (int) –

  • angle (Union[int, float]) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

Return type

T

replace() → T[source]

Replace the underlying faces with the selection.

Parameters

self (T) –

Return type

T

reset() → T[source]

Reset current selection.

Parameters

self (T) –

Return type

T

segment(l: Union[int, float], a: Union[int, float], tag: Optional[str] = None, forConstruction: bool = False) → T[source]
segment(p2: Union[Vector, Tuple[Union[int, float], Union[int, float]]], tag: Optional[str] = None, forConstruction: bool = False) → T
segment(p1: Union[Vector, Tuple[Union[int, float], Union[int, float]]], p2: Union[Vector, Tuple[Union[int, float], Union[int, float]]], tag: Optional[str] = None, forConstruction: bool = False) → T

Construct a segment.

Parameters

  • self (T) –

  • p1 (Union[Vector, Tuple[Union[int, float], Union[int, float]]]) –

  • p2 (Union[Vector, Tuple[Union[int, float], Union[int, float]]]) –

  • tag (Optional[str]) –

  • forConstruction (bool) –

Return type

T

select(*tags: str) → T[source]

Select based on tags.

Parameters

  • self (T) –

  • tags (str) –

Return type

T

slot(w: Union[int, float], h: Union[int, float], angle: Union[int, float] = 0, mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None) → T[source]

Construct a slot-shaped face.

Parameters

  • self (T) –

  • w (Union[int, float]) –

  • h (Union[int, float]) –

  • angle (Union[int, float]) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

Return type

T

solve() → T[source]

Solve current constraints and update edge positions.

Parameters

self (T) –

Return type

T

sort(key: Callable[[Union[Shape, Location]], Any]) → T[source]

Sort items using a callable.

Parameters

  • self (T) –

  • key (Callable[[Union[Shape, Location]], Any]) – Callable to be used for sorting.

Returns

Sketch object with items sorted.

Return type

T

spline(pts: Iterable[Union[Vector, Tuple[Union[int, float], Union[int, float]]]], tag: Optional[str] = None, forConstruction: bool = False) → T[source]
spline(pts: Iterable[Union[Vector, Tuple[Union[int, float], Union[int, float]]]], tangents: Optional[Iterable[Union[Vector, Tuple[Union[int, float], Union[int, float]]]]], periodic: bool, tag: Optional[str] = None, forConstruction: bool = False) → T

Construct a spline edge.

Parameters

  • self (T) –

  • pts (Iterable[Union[Vector, Tuple[Union[int, float], Union[int, float]]]]) –

  • tangents (Optional[Iterable[Union[Vector, Tuple[Union[int, float], Union[int, float]]]]]) –

  • periodic (bool) –

  • tag (Optional[str]) –

  • forConstruction (bool) –

Return type

T

subtract() → T[source]

Subtract selection from the underlying faces.

Parameters

self (T) –

Return type

T

tag(tag: str) → T[source]

Tag current selection.

Parameters

  • self (T) –

  • tag (str) –

Return type

T

trapezoid(w: Union[int, float], h: Union[int, float], a1: Union[int, float], a2: Optional[float] = None, angle: Union[int, float] = 0, mode: Literal['a', 's', 'i', 'c', 'r'] = 'a', tag: Optional[str] = None) → T[source]

Construct a trapezoidal face.

Parameters

  • self (T) –

  • w (Union[int, float]) –

  • h (Union[int, float]) –

  • a1 (Union[int, float]) –

  • a2 (Optional[float]) –

  • angle (Union[int, float]) –

  • mode (Literal['a', 's', 'i', 'c', 'r']) –

  • tag (Optional[str]) –

Return type

T

val() → Union[Shape, Location][source]

Return the first selected item, underlying compound or first edge.

Parameters

self (T) –

Return type

Union[Shape, Location]

vals() → List[Union[Shape, Location]][source]

Return all selected items, underlying compound or all edges.

Parameters

self (T) –

Return type

List[Union[Shape, Location]]

vertices(s: Optional[Union[str, Selector]] = None, tag: Optional[str] = None) → T[source]

Select vertices.

Parameters

  • self (T) –

  • s (Optional[Union[str, Selector]]) –

  • tag (Optional[str]) –

Return type

T

wires(s: Optional[Union[str, Selector]] = None, tag: Optional[str] = None) → T[source]

Select wires.

Parameters

  • self (T) –

  • s (Optional[Union[str, Selector]]) –

  • tag (Optional[str]) –

Return type

T

class cadquery.Solid(obj: TopoDS_Shape)[source]

Bases: Shape, Mixin3D

a single solid

Parameters

obj (TopoDS_Shape) –

classmethod extrudeLinear(outerWire: Wire, innerWires: List[Wire], vecNormal: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], taper: Union[float, int] = 0) → Solid[source]
classmethod extrudeLinear(face: Face, vecNormal: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], taper: Union[float, int] = 0) → Solid

Attempt to extrude the list of wires into a prismatic solid in the provided direction

Parameters

  • outerWire (Wire) – the outermost wire

  • innerWires (List[Wire]) – a list of inner wires

  • vecNormal (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – a vector along which to extrude the wires

  • taper (Union[float, int]) – taper angle, default=0

Returns

a Solid object

Return type

Solid

The wires must not intersect

Extruding wires is very non-trivial. Nested wires imply very different geometry, and there are many geometries that are invalid. In general, the following conditions must be met:

  • all wires must be closed

  • there cannot be any intersecting or self-intersecting wires

  • wires must be listed from outside in

  • more than one levels of nesting is not supported reliably

This method will attempt to sort the wires, but there is much work remaining to make this method reliable.

classmethod extrudeLinearWithRotation(outerWire: Wire, innerWires: List[Wire], vecCenter: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], vecNormal: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], angleDegrees: Union[float, int]) → Solid[source]
classmethod extrudeLinearWithRotation(face: Face, vecCenter: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], vecNormal: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], angleDegrees: Union[float, int]) → Solid

Creates a ‘twisted prism’ by extruding, while simultaneously rotating around the extrusion vector.

Though the signature may appear to be similar enough to extrudeLinear to merit combining them, the construction methods used here are different enough that they should be separate.

At a high level, the steps followed are:

  1. accept a set of wires

  2. create another set of wires like this one, but which are transformed and rotated

  3. create a ruledSurface between the sets of wires

  4. create a shell and compute the resulting object

Parameters

  • outerWire (Wire) – the outermost wire

  • innerWires (List[Wire]) – a list of inner wires

  • vecCenter (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – the center point about which to rotate. the axis of rotation is defined by vecNormal, located at vecCenter.

  • vecNormal (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – a vector along which to extrude the wires

  • angleDegrees (Union[float, int]) – the angle to rotate through while extruding

Returns

a Solid object

Return type

Solid

classmethod interpPlate(surf_edges, surf_pts, thickness, degree=3, nbPtsOnCur=15, nbIter=2, anisotropy=False, tol2d=1e-05, tol3d=0.0001, tolAng=0.01, tolCurv=0.1, maxDeg=8, maxSegments=9) → Union[Solid, Face][source]

Returns a plate surface that is ‘thickness’ thick, enclosed by ‘surf_edge_pts’ points, and going through ‘surf_pts’ points.

Parameters

  • surf_edges – list of [x,y,z] float ordered coordinates or list of ordered or unordered wires

  • surf_pts – list of [x,y,z] float coordinates (uses only edges if [])

  • thickness – thickness may be negative or positive depending on direction, (returns 2D surface if 0)

  • degree – >=2

  • nbPtsOnCur – number of points on curve >= 15

  • nbIter – number of iterations >= 2

  • anisotropy – bool Anisotropy

  • tol2d – 2D tolerance >0

  • tol3d – 3D tolerance >0

  • tolAng – angular tolerance

  • tolCurv – tolerance for curvature >0

  • maxDeg – highest polynomial degree >= 2

  • maxSegments – greatest number of segments >= 2

Return type

Union[Solid, Face]

static isSolid(obj: Shape) → bool[source]

Returns true if the object is a solid, false otherwise

Parameters

obj (Shape) –

Return type

bool

classmethod makeBox(length,width,height,[pnt,dir]) -- Make a box located in pnt with the dimensions (length,width,height)[source]

By default pnt=Vector(0,0,0) and dir=Vector(0,0,1)

Parameters

  • length (float) –

  • width (float) –

  • height (float) –

  • pnt (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • dir (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

Return type

Solid

classmethod makeCone(radius1: float, radius2: float, height: float, pnt: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 0.0), dir: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 1.0), angleDegrees: float = 360) → Solid[source]

Make a cone with given radii and height By default pnt=Vector(0,0,0), dir=Vector(0,0,1) and angle=360

Parameters

  • radius1 (float) –

  • radius2 (float) –

  • height (float) –

  • pnt (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • dir (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • angleDegrees (float) –

Return type

Solid

classmethod makeCylinder(radius: float, height: float, pnt: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 0.0), dir: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 1.0), angleDegrees: float = 360) → Solid[source]

makeCylinder(radius,height,[pnt,dir,angle]) – Make a cylinder with a given radius and height By default pnt=Vector(0,0,0),dir=Vector(0,0,1) and angle=360

Parameters

  • radius (float) –

  • height (float) –

  • pnt (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • dir (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • angleDegrees (float) –

Return type

Solid

classmethod makeLoft(listOfWire: List[Wire], ruled: bool = False) → Solid[source]

makes a loft from a list of wires The wires will be converted into faces when possible– it is presumed that nobody ever actually wants to make an infinitely thin shell for a real FreeCADPart.

Parameters

  • listOfWire (List[Wire]) –

  • ruled (bool) –

Return type

Solid

classmethod makeSolid(shell: Shell) → Solid[source]

Makes a solid from a single shell.

Parameters

shell (Shell) –

Return type

Solid

classmethod makeSphere(radius: float, pnt: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 0.0), dir: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 1.0), angleDegrees1: float = 0, angleDegrees2: float = 90, angleDegrees3: float = 360) → Shape[source]

Make a sphere with a given radius By default pnt=Vector(0,0,0), dir=Vector(0,0,1), angle1=0, angle2=90 and angle3=360

Parameters

  • radius (float) –

  • pnt (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • dir (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • angleDegrees1 (float) –

  • angleDegrees2 (float) –

  • angleDegrees3 (float) –

Return type

Shape

classmethod makeTorus(radius1: float, radius2: float, pnt: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 0.0), dir: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 1.0), angleDegrees1: float = 0, angleDegrees2: float = 360) → Solid[source]

makeTorus(radius1,radius2,[pnt,dir,angle1,angle2,angle]) – Make a torus with a given radii and angles By default pnt=Vector(0,0,0),dir=Vector(0,0,1),angle1=0 ,angle1=360 and angle=360

Parameters

  • radius1 (float) –

  • radius2 (float) –

  • pnt (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • dir (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • angleDegrees1 (float) –

  • angleDegrees2 (float) –

Return type

Solid

classmethod makeWedge(dx: float, dy: float, dz: float, xmin: float, zmin: float, xmax: float, zmax: float, pnt: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 0.0), dir: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 1.0)) → Solid[source]

Make a wedge located in pnt By default pnt=Vector(0,0,0) and dir=Vector(0,0,1)

Parameters

  • dx (float) –

  • dy (float) –

  • dz (float) –

  • xmin (float) –

  • zmin (float) –

  • xmax (float) –

  • zmax (float) –

  • pnt (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • dir (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

Return type

Solid

classmethod revolve(outerWire: Wire, innerWires: List[Wire], angleDegrees: Union[float, int], axisStart: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], axisEnd: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → Solid[source]
classmethod revolve(face: Face, angleDegrees: Union[float, int], axisStart: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], axisEnd: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → Solid

Attempt to revolve the list of wires into a solid in the provided direction

Parameters

  • outerWire (Wire) – the outermost wire

  • innerWires (List[Wire]) – a list of inner wires

  • angleDegrees (float, anything less than 360 degrees will leave the shape open) – the angle to revolve through.

  • axisStart (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – the start point of the axis of rotation

  • axisEnd (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – the end point of the axis of rotation

Returns

a Solid object

Return type

Solid

The wires must not intersect

  • all wires must be closed

  • there cannot be any intersecting or self-intersecting wires

  • wires must be listed from outside in

  • more than one levels of nesting is not supported reliably

  • the wire(s) that you’re revolving cannot be centered

This method will attempt to sort the wires, but there is much work remaining to make this method reliable.

classmethod sweep(face: Face, path: Union[Wire, Edge], makeSolid: bool = True, isFrenet: bool = False, mode: Optional[Union[Vector, Wire, Edge]] = None, transitionMode: Literal['transformed', 'round', 'right'] = 'transformed') → Shape[source]
classmethod sweep(outerWire: Wire, innerWires: List[Wire], path: Union[Wire, Edge], makeSolid: bool = True, isFrenet: bool = False, mode: Optional[Union[Vector, Wire, Edge]] = None, transitionMode: Literal['transformed', 'round', 'right'] = 'transformed') → Shape

Attempt to sweep the list of wires into a prismatic solid along the provided path

Parameters

  • outerWire (Wire) – the outermost wire

  • innerWires (List[Wire]) – a list of inner wires

  • path (Union[Wire, Edge]) – The wire to sweep the face resulting from the wires over

  • makeSolid (bool) – return Solid or Shell (default True)

  • isFrenet (bool) – Frenet mode (default False)

  • mode (Optional[Union[Vector, Wire, Edge]]) – additional sweep mode parameters

  • transitionMode (Literal['transformed', 'round', 'right']) – handling of profile orientation at C1 path discontinuities. Possible values are {‘transformed’,’round’, ‘right’} (default: ‘right’).

Returns

a Solid object

Return type

Shape

classmethod sweep_multi(profiles: Iterable[Union[Wire, Face]], path: Union[Wire, Edge], makeSolid: bool = True, isFrenet: bool = False, mode: Optional[Union[Vector, Wire, Edge]] = None) → Solid[source]

Multi section sweep. Only single outer profile per section is allowed.

Parameters

  • profiles (Iterable[Union[Wire, Face]]) – list of profiles

  • path (Union[Wire, Edge]) – The wire to sweep the face resulting from the wires over

  • mode (Optional[Union[Vector, Wire, Edge]]) – additional sweep mode parameters.

  • makeSolid (bool) –

  • isFrenet (bool) –

Returns

a Solid object

Return type

Solid

class cadquery.StringSyntaxSelector(selectorString)[source]

Bases: Selector

Filter lists objects using a simple string syntax. All of the filters available in the string syntax are also available ( usually with more functionality ) through the creation of full-fledged selector objects. see Selector and its subclasses

Filtering works differently depending on the type of object list being filtered.

Parameters

selectorString – A two-part selector string, [selector][axis]

Returns

objects that match the specified selector

*Modifiers* are ('|','+','-','<','>','%')

|

parallel to ( same as ParallelDirSelector ). Can return multiple objects.

#

perpendicular to (same as PerpendicularDirSelector )

+

positive direction (same as DirectionSelector )

-

negative direction (same as DirectionSelector )

>

maximize (same as DirectionMinMaxSelector with directionMax=True)

<

minimize (same as DirectionMinMaxSelector with directionMax=False )

%

curve/surface type (same as TypeSelector)

*axisStrings* are: X,Y,Z,XY,YZ,XZ or (x,y,z) which defines an arbitrary direction

It is possible to combine simple selectors together using logical operations. The following operations are supported

and

Logical AND, e.g. >X and >Y

or

Logical OR, e.g. |X or |Y

not

Logical NOT, e.g. not #XY

exc(ept)

Set difference (equivalent to AND NOT): |X exc >Z

Finally, it is also possible to use even more complex expressions with nesting and arbitrary number of terms, e.g.

(not >X[0] and #XY) or >XY[0]

Selectors are a complex topic: see Selectors Reference for more information

__init__(selectorString)[source]

Feed the input string through the parser and construct an relevant complex selector object

filter(objectList: Sequence[Shape])[source]

Filter give object list through th already constructed complex selector object

Parameters

objectList (Sequence[Shape]) –

class cadquery.TypeSelector(typeString: str)[source]

Bases: Selector

Selects objects having the prescribed geometry type.

Applicability:

Faces: PLANE, CYLINDER, CONE, SPHERE, TORUS, BEZIER, BSPLINE, REVOLUTION, EXTRUSION, OFFSET, OTHER Edges: LINE, CIRCLE, ELLIPSE, HYPERBOLA, PARABOLA, BEZIER, BSPLINE, OFFSET, OTHER

You can use the string selector syntax. For example this:

CQ(aCube).faces(TypeSelector("PLANE"))

will select 6 faces, and is equivalent to:

CQ(aCube).faces("%PLANE")
Parameters

typeString (str) –

__init__(typeString: str)[source]
Parameters

typeString (str) –

filter(objectList: Sequence[Shape]) → List[Shape][source]

Filter the provided list.

The default implementation returns the original list unfiltered.

Parameters

objectList (list of OCCT primitives) – list to filter

Returns

filtered list

Return type

List[Shape]

class cadquery.Vector(x: float, y: float, z: float)[source]
class cadquery.Vector(x: float, y: float)
class cadquery.Vector(v: Vector)
class cadquery.Vector(v: Sequence[float])
class cadquery.Vector(v: Union[gp_Vec, gp_Pnt, gp_Dir, gp_XYZ])
class cadquery.Vector

Bases: object

Create a 3-dimensional vector

Parameters

args – a 3D vector, with x-y-z parts.

you can either provide:

  • nothing (in which case the null vector is return)

  • a gp_Vec

  • a vector ( in which case it is copied )

  • a 3-tuple

  • a 2-tuple (z assumed to be 0)

  • three float values: x, y, and z

  • two float values: x,y

Center() → Vector[source]

Return the vector itself

The center of myself is myself. Provided so that vectors, vertices, and other shapes all support a common interface, when Center() is requested for all objects on the stack.

Return type

Vector

__eq__(other: Vector) → bool[source]

Return self==value.

Parameters

other (Vector) –

Return type

bool

__hash__ = None
__init__(x: float, y: float, z: float) → None[source]
__init__(x: float, y: float) → None
__init__(v: Vector) → None
__init__(v: Sequence[float]) → None
__init__(v: Union[gp_Vec, gp_Pnt, gp_Dir, gp_XYZ]) → None
__init__() → None
__repr__() → str[source]

Return repr(self).

Return type

str

__str__() → str[source]

Return str(self).

Return type

str

__weakref__

list of weak references to the object (if defined)

multiply(scale: float) → Vector[source]

Return a copy multiplied by the provided scalar

Parameters

scale (float) –

Return type

Vector

normalized() → Vector[source]

Return a normalized version of this vector

Return type

Vector

projectToLine(line: Vector) → Vector[source]

Returns a new vector equal to the projection of this Vector onto the line represented by Vector <line>

Parameters

  • args – Vector

  • line (Vector) –

Return type

Vector

Returns the projected vector.

projectToPlane(plane: Plane) → Vector[source]

Vector is projected onto the plane provided as input.

Parameters

  • args – Plane object

  • plane (Plane) –

Return type

Vector

Returns the projected vector.

class cadquery.Vertex(obj: TopoDS_Shape, forConstruction: bool = False)[source]

Bases: Shape

A Single Point in Space

Parameters

  • obj (TopoDS_Shape) –

  • forConstruction (bool) –

Center() → Vector[source]

The center of a vertex is itself!

Return type

Vector

__init__(obj: TopoDS_Shape, forConstruction: bool = False)[source]

Create a vertex

Parameters

  • obj (TopoDS_Shape) –

  • forConstruction (bool) –

class cadquery.Wire(obj: TopoDS_Shape)[source]

Bases: Shape, Mixin1D

A series of connected, ordered Edges, that typically bounds a Face

Parameters

obj (TopoDS_Shape) –

Vertices() → List[Vertex][source]

Ordered list of vertices of the wire.

Return type

List[Vertex]

__iter__() → Iterator[Edge][source]

Iterate over edges in an ordered way.

Return type

Iterator[Edge]

classmethod assembleEdges(listOfEdges: Iterable[Edge]) → Wire[source]

Attempts to build a wire that consists of the edges in the provided list

Parameters

  • cls –

  • listOfEdges (Iterable[Edge]) – a list of Edge objects. The edges are not to be consecutive.

Returns

a wire with the edges assembled

Return type

Wire

BRepBuilderAPI_MakeWire::Error() values:

  • BRepBuilderAPI_WireDone = 0

  • BRepBuilderAPI_EmptyWire = 1

  • BRepBuilderAPI_DisconnectedWire = 2

  • BRepBuilderAPI_NonManifoldWire = 3

chamfer2D(d: float, vertices: Iterable[Vertex]) → Wire[source]

Apply 2D chamfer to a wire

Parameters

  • d (float) –

  • vertices (Iterable[Vertex]) –

Return type

Wire

close() → Wire[source]

Close a Wire

Return type

Wire

classmethod combine(listOfWires: Iterable[Union[Wire, Edge]], tol: float = 1e-09) → List[Wire][source]

Attempt to combine a list of wires and edges into a new wire.

Parameters

  • cls –

  • listOfWires (Iterable[Union[Wire, Edge]]) –

  • tol (float) – default 1e-9

Returns

List[Wire]

Return type

List[Wire]

fillet(radius: float, vertices: Optional[Iterable[Vertex]] = None) → Wire[source]

Apply 2D or 3D fillet to a wire

Parameters

  • radius (float) – the radius of the fillet, must be > zero

  • vertices (Optional[Iterable[Vertex]]) – Optional list of vertices to fillet. By default all vertices are fillet.

Returns

A wire with filleted corners

Return type

Wire

fillet2D(radius: float, vertices: Iterable[Vertex]) → Wire[source]

Apply 2D fillet to a wire

Parameters

  • radius (float) –

  • vertices (Iterable[Vertex]) –

Return type

Wire

classmethod makeCircle(radius: float, center: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], normal: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) → Wire[source]

Makes a Circle centered at the provided point, having normal in the provided direction

Parameters

  • radius (float) – floating point radius of the circle, must be > 0

  • center (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – vector representing the center of the circle

  • normal (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – vector representing the direction of the plane the circle should lie in

Return type

Wire

classmethod makeEllipse(x_radius: float, y_radius: float, center: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], normal: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], xDir: Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]], angle1: float = 360.0, angle2: float = 360.0, rotation_angle: float = 0.0, closed: bool = True) → Wire[source]

Makes an Ellipse centered at the provided point, having normal in the provided direction

Parameters

  • x_radius (float) – floating point major radius of the ellipse (x-axis), must be > 0

  • y_radius (float) – floating point minor radius of the ellipse (y-axis), must be > 0

  • center (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – vector representing the center of the circle

  • normal (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) – vector representing the direction of the plane the circle should lie in

  • angle1 (float) – start angle of arc

  • angle2 (float) – end angle of arc

  • rotation_angle (float) – angle to rotate the created ellipse / arc

  • xDir (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • closed (bool) –

Return type

Wire

classmethod makeHelix(pitch: float, height: float, radius: float, center: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 0.0), dir: ~typing.Union[~cadquery.occ_impl.geom.Vector, ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float]], ~typing.Tuple[~typing.Union[int, float], ~typing.Union[int, float], ~typing.Union[int, float]]] = Vector: (0.0, 0.0, 1.0), angle: float = 360.0, lefthand: bool = False) → Wire[source]

Make a helix with a given pitch, height and radius By default a cylindrical surface is used to create the helix. If the fourth parameter is set (the apex given in degree) a conical surface is used instead’

Parameters

  • pitch (float) –

  • height (float) –

  • radius (float) –

  • center (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • dir (Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]) –

  • angle (float) –

  • lefthand (bool) –

Return type

Wire

classmethod makePolygon(listOfVertices: Iterable[Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]], forConstruction: bool = False, close: bool = False) → Wire[source]

Construct a polygonal wire from points.

Parameters

  • listOfVertices (Iterable[Union[Vector, Tuple[Union[int, float], Union[int, float]], Tuple[Union[int, float], Union[int, float], Union[int, float]]]]) –

  • forConstruction (bool) –

  • close (bool) –

Return type

Wire

offset2D(d: float, kind: Literal['arc', 'intersection', 'tangent'] = 'arc') → List[Wire][source]

Offsets a planar wire

Parameters

  • d (float) –

  • kind (Literal['arc', 'intersection', 'tangent']) –

Return type

List[Wire]

stitch(other: Wire) → Wire[source]

Attempt to stitch wires

Parameters

other (Wire) –

Return type

Wire

class cadquery.Workplane(obj: Union[Vector, Location, Shape, Sketch])[source]
class cadquery.Workplane(inPlane: Union[Plane, str] = 'XY', origin: Union[Tuple[float, float], Tuple[float, float, float], Vector] = (0, 0, 0), obj: Optional[Union[Vector, Location, Shape, Sketch]] = None)

Bases: object

Defines a coordinate system in space, in which 2D coordinates can be used.

Parameters

  • plane (a Plane object, or a string in (XY|YZ|XZ|front|back|top|bottom|left|right)) – the plane in which the workplane will be done

  • origin (a 3-tuple in global coordinates, or None to default to the origin) – the desired origin of the new workplane

  • obj (a CAD primitive, or None to use the centerpoint of the plane as the initial stack value.) – an object to use initially for the stack

Raises

ValueError if the provided plane is not a plane, a valid named workplane

Returns

A Workplane object, with coordinate system matching the supplied plane.

The most common use is:

s = Workplane("XY")

After creation, the stack contains a single point, the origin of the underlying plane, and the current point is on the origin.

Note

You can also create workplanes on the surface of existing faces using workplane()

__add__(other: Union[Workplane, Solid, Compound]) → T[source]

Syntactic sugar for union.

Notice that r = a + b is equivalent to r = a.union(b) and r = a | b.

Parameters
Return type

T

__and__(other: Union[Workplane, Solid, Compound]) → T[source]

Syntactic sugar for intersect.

Notice that r = a & b is equivalent to r = a.intersect(b).

Example:

Box = Workplane("XY").box(1, 1, 1, centered=(False, False, False))
Sphere = Workplane("XY").sphere(1)
result = Box & Sphere
Parameters
Return type

T

__init__(obj: Union[Vector, Location, Shape, Sketch]) → None[source]
__init__(inPlane: Union[Plane, str] = 'XY', origin: Union[Tuple[float, float], Tuple[float, float, float], Vector] = (0, 0, 0), obj: Optional[Union[Vector, Location, Shape, Sketch]] = None) → None

make a workplane from a particular plane

Parameters

  • inPlane (a Plane object, or a string in (XY|YZ|XZ|front|back|top|bottom|left|right)) – the plane in which the workplane will be done

  • origin (a 3-tuple in global coordinates, or None to default to the origin) – the desired origin of the new workplane

  • obj (a CAD primitive, or None to use the centerpoint of the plane as the initial stack value.) – an object to use initially for the stack

Raises

ValueError if the provided plane is not a plane, or one of XY|YZ|XZ

Returns

A Workplane object, with coordinate system matching the supplied plane.

The most common use is:

s = Workplane("XY")

After creation, the stack contains a single point, the origin of the underlying plane, and the current point is on the origin.

__iter__() → Iterator[Shape][source]

Special method for iterating over Shapes in objects

Parameters

self (T) –

Return type

Iterator[Shape]

__mul__(other: Union[Workplane, Solid, Compound]) → T[source]

Syntactic sugar for intersect.

Notice that r = a * b is equivalent to r = a.intersect(b).

Example:

Box = Workplane("XY").box(1, 1, 1, centered=(False, False, False))
Sphere = Workplane("XY").sphere(1)
result = Box * Sphere
Parameters
Return type

T

__or__(other: Union[Workplane, Solid, Compound]) → T[source]

Syntactic sugar for union.

Notice that r = a | b is equivalent to r = a.union(b) and r = a + b.

Example:

Box = Workplane("XY").box(1, 1, 1, centered=(False, False, False))
Sphere = Workplane("XY").sphere(1)
result = Box | Sphere
Parameters
Return type

T

__sub__(other: Union[Workplane, Solid, Compound]) → T[source]

Syntactic sugar for cut.

Notice that r = a - b is equivalent to r = a.cut(b).

Example:

Box = Workplane("XY").box(1, 1, 1, centered=(False, False, False))
Sphere = Workplane("XY").sphere(1)
result = Box - Sphere
Parameters
Return type

T

__truediv__(other: Union[Workplane, Solid, Compound]) → T[source]

Syntactic sugar for intersect.

Notice that r = a / b is equivalent to r = a.split(b).

Example:

Box = Workplane("XY").box(1, 1, 1, centered=(False, False, False))
Sphere = Workplane("XY").sphere(1)
result = Box / Sphere
Parameters
Return type

T

__weakref__

list of weak references to the object (if defined)

add(obj: Workplane) → T[source]
add(obj: Union[Vector, Location, Shape, Sketch]) → T
add(obj: Iterable[Union[Vector, Location, Shape, Sketch]]) → T

Adds an object or a list of objects to the stack

Parameters

obj (a Workplane, CAD primitive, or list of CAD primitives) – an object to add

Returns

a Workplane with the requested operation performed

If a Workplane object, the values of that object’s stack are added. If a list of cad primitives, they are all added. If a single CAD primitive then it is added.

Used in rare cases when you need to combine the results of several CQ results into a single Workplane object.

all() → List[T][source]

Return a list of all CQ objects on the stack.

useful when you need to operate on the elements individually.

Contrast with vals, which returns the underlying objects for all of the items on the stack

Parameters

self (T) –

Return type

List[T]

ancestors(kind: Literal['Vertex', 'Edge', 'Wire', 'Face', 'Shell', 'Solid', 'CompSolid', 'Compound'], tag: Optional[str] = None) → T[source]

Select topological ancestors.

Parameters

  • self (T) –

  • kind (Literal['Vertex', 'Edge', 'Wire', 'Face', 'Shell', 'Solid', 'CompSolid', 'Compound']) – kind of ancestor, e.g. “Face” or “Edge”

  • tag (Optional[str]) – if set, search the tagged object instead of self

Returns

a Workplane object whose stack contains selected ancestors.

Return type

T

apply(f: Callable[[Iterable[Union[Vector, Location, Shape, Sketch]]], Iterable[Union[Vector, Location, Shape, Sketch]]]) → T[source]

Apply a callable to all items at once.

Parameters
Returns

Workplane object with f applied to all items.

Return type

T

bezier(listOfXYTuple: Iterable[Union[Tuple[float, float], Tuple[float, float, float], Vector]], forConstruction: bool = False, includeCurrent: bool = False, makeWire: bool = False) → T[source]

Make a cubic Bézier curve by the provided points (2D or 3D).

Parameters

  • self (T) –

  • listOfXYTuple (Iterable[Union[Tuple[float, float], Tuple[float, float, float], Vector]]) – Bezier control points and end point. All points except the last point are Bezier control points, and the last point is the end point

  • includeCurrent (bool) – Use the current point as a starting point of the curve

  • makeWire (bool) – convert the resulting bezier edge to a wire

  • forConstruction (bool) –

Returns

a Workplane object with the current point at the end of the bezier

Return type

T

The Bézier Will begin at either current point or the first point of listOfXYTuple, and end with the last point of listOfXYTuple

box(length: float, width: float, height: float, centered: Union[bool, Tuple[bool, bool, bool]] = True, combine: Union[bool, Literal['cut', 'a', 's']] = True, clean: bool = True) → T[source]

Return a 3d box with specified dimensions for each object on the stack.

Parameters

  • self (T) –

  • length (float) – box size in X direction

  • width (float) – box size in Y direction

  • height (float) – box size in Z direction

  • centered (Union[bool, Tuple[bool, bool, bool]]) – If True, the box will be centered around the reference point. If False, the corner of the box will be on the reference point and it will extend in the positive x, y and z directions. Can also use a 3-tuple to specify centering along each axis.

  • combine (Union[bool, Literal['cut', 'a', 's']]) – should the results be combined with other solids on the stack (and each other)?

  • clean (bool) – call clean() afterwards to have a clean shape

Return type

T

One box is created for each item on the current stack. If no items are on the stack, one box using the current workplane center is created.

If combine is true, the result will be a single object on the stack. If a solid was found in the chain, the result is that solid with all boxes produced fused onto it otherwise, the result is the combination of all the produced boxes.

If combine is false, the result will be a list of the boxes produced.

Most often boxes form the basis for a part:

# make a single box with lower left corner at origin
s = Workplane().box(1, 2, 3, centered=False)

But sometimes it is useful to create an array of them:

# create 4 small square bumps on a larger base plate:
s = (
    Workplane()
    .box(4, 4, 0.5)
    .faces(">Z")
    .workplane()
    .rect(3, 3, forConstruction=True)
    .vertices()
    .box(0.25, 0.25, 0.25, combine=True)
)
cboreHole(diameter: float, cboreDiameter: float, cboreDepth: float, depth: Optional[float] = None, clean: bool = True) → T[source]

Makes a counterbored hole for each item on the stack.

Parameters

  • self (T) –

  • diameter (float) – the diameter of the hole

  • cboreDiameter (float) – the diameter of the cbore, must be greater than hole diameter

  • cboreDepth (float > 0) – depth of the counterbore

  • depth (float > 0 or None to drill thru the entire part) – the depth of the hole

  • clean (bool) – call clean() afterwards to have a clean shape

Return type

T

The surface of the hole is at the current workplane plane.

One hole is created for each item on the stack. A very common use case is to use a construction rectangle to define the centers of a set of holes, like so:

s = (
    Workplane()
    .box(2, 4, 0.5)
    .faces(">Z")
    .workplane()
    .rect(1.5, 3.5, forConstruction=True)
    .vertices()
    .cboreHole(0.125, 0.25, 0.125, depth=None)
)

This sample creates a plate with a set of holes at the corners.

Plugin Note: this is one example of the power of plugins. Counterbored holes are quite time consuming to create, but are quite easily defined by users.

see cskHole() to make countersinks instead of counterbores

center(x: float, y: float) → T[source]

Shift local coordinates to the specified location.

The location is specified in terms of local coordinates.

Parameters

  • self (T) –

  • x (float) – the new x location

  • y (float) – the new y location

Returns

the Workplane object, with the center adjusted.

Return type

T

The current point is set to the new center. This method is useful to adjust the center point after it has been created automatically on a face, but not where you’d like it to be.

In this example, we adjust the workplane center to be at the corner of a cube, instead of the center of a face, which is the default:

# this workplane is centered at x=0.5,y=0.5, the center of the upper face
s = Workplane().box(1, 1, 1).faces(">Z").workplane()

s = s.center(-0.5, -0.5)  # move the center to the corner
t = s.circle(0.25).extrude(0.2)
assert t.faces().size() == 9  # a cube with a cylindrical nub at the top right corner

The result is a cube with a round boss on the corner

chamfer(length: float, length2: Optional[float] = None) → T[source]

Chamfers a solid on the selected edges.

The edges on the stack are chamfered. The solid to which the edges belong must be in the parent chain of the selected edges.

Optional parameter length2 can be supplied with a different value than length for a chamfer that is shorter on one side longer on the other side.

Parameters

  • self (T) –

  • length (float) – the length of the chamfer, must be greater than zero

  • length2 (Optional[float]) – optional parameter for asymmetrical chamfer

Raises

  • ValueError – if at least one edge is not selected

  • ValueError – if the solid containing the edge is not in the chain

Returns

CQ object with the resulting solid selected.

Return type

T

This example will create a unit cube, with the top edges chamfered:

s = Workplane("XY").box(1, 1, 1).faces("+Z").chamfer(0.1)

This example will create chamfers longer on the sides:

s = Workplane("XY").box(1, 1, 1).faces("+Z").chamfer(0.2, 0.1)
circle(radius: float, forConstruction: bool = False) → T[source]

Make a circle for each item on the stack.

Parameters

  • self (T) –

  • radius (float) – radius of the circle

  • forConstruction (true if the wires are for reference, false if they are creating part geometry) – should the new wires be reference geometry only?

Returns

a new CQ object with the created wires on the stack

Return type

T

A common use case is to use a for-construction rectangle to define the centers of a hole pattern:

s = Workplane().rect(4.0, 4.0, forConstruction=True).vertices().circle(0.25)

Creates 4 circles at the corners of a square centered on the origin. Another common case is to use successive circle() calls to create concentric circles. This works because the center of a circle is its reference point:

s = Workplane().circle(2.0).circle(1.0)

Creates two concentric circles, which when extruded will form a ring.

Future Enhancements:

better way to handle forConstruction project points not in the workplane plane onto the workplane plane

clean() → T[source]

Cleans the current solid by removing unwanted edges from the faces.

Normally you don’t have to call this function. It is automatically called after each related operation. You can disable this behavior with clean=False parameter if method has any. In some cases this can improve performance drastically but is generally dis-advised since it may break some operations such as fillet.

Note that in some cases where lots of solid operations are chained, clean() may actually improve performance since the shape is ‘simplified’ at each step and thus next operation is easier.

Also note that, due to limitation of the underlying engine, clean may fail to produce a clean output in some cases such as spherical faces.

Parameters

self (T) –

Return type

T

close() → T[source]

End construction, and attempt to build a closed wire.

Returns

a CQ object with a completed wire on the stack, if possible.

Parameters

self (T) –

Return type

T

After 2D (or 3D) drafting with methods such as lineTo, threePointArc, tangentArcPoint and polyline, it is necessary to convert the edges produced by these into one or more wires.

When a set of edges is closed, CadQuery assumes it is safe to build the group of edges into a wire. This example builds a simple triangular prism:

s = Workplane().lineTo(1, 0).lineTo(1, 1).close().extrude(0.2)
combine(clean: bool = True, glue: bool = False, tol: Optional[float] = None) → T[source]

Attempts to combine all of the items on the stack into a single item.

WARNING: all of the items must be of the same type!

Parameters

  • self (T) –

  • clean (bool) – call clean() afterwards to have a clean shape

  • glue (bool) – use a faster gluing mode for non-overlapping shapes (default False)

  • tol (Optional[float]) – tolerance value for fuzzy bool operation mode (default None)

Raises

ValueError if there are no items on the stack, or if they cannot be combined

Returns

a CQ object with the resulting object selected

Return type

T

combineSolids(otherCQToCombine: Optional[Workplane] = None) → Workplane[source]

!!!DEPRECATED!!! use union() Combines all solids on the current stack, and any context object, together into a single object.

After the operation, the returned solid is also the context solid.

Parameters

otherCQToCombine (Optional[Workplane]) – another CadQuery to combine.

Returns

a CQ object with the resulting combined solid on the stack.

Return type

Workplane

Most of the time, both objects will contain a single solid, which is combined and returned on the stack of the new object.

compounds(selector: Optional[Union[str, Selector]] = None, tag: Optional[str] = None) → T[source]

Select compounds on the stack, optionally filtering the selection. If there are multiple objects on the stack, they are collected and a list of all the distinct compounds is returned.

Parameters

  • self (T) –

  • selector (Optional[Union[str, Selector]]) – optional Selector object, or string selector expression (see StringSyntaxSelector)

  • tag (Optional[str]) – if set, search the tagged object instead of self

Returns

a CQ object whose stack contains all of the distinct compounds of all objects on the current stack, filtered by the provided selector.

Return type

T

A compound contains multiple CAD primitives that resulted from a single operation, such as a union, cut, split, or fillet. Compounds can contain multiple edges, wires, or solids.

consolidateWires() → T[source]

Attempt to consolidate wires on the stack into a single. If possible, a new object with the results are returned. if not possible, the wires remain separated

Parameters

self (T) –

Return type

T

copyWorkplane(obj: T) → T[source]

Copies the workplane from obj.

Parameters

obj (a CQ object) – an object to copy the workplane from

Returns

a CQ object with obj’s workplane

Return type

T

cskHole(diameter: float, cskDiameter: float, cskAngle: float, depth: Optional[float] = None, clean: bool = True) → T[source]

Makes a countersunk hole for each item on the stack.

Parameters

  • self (T) –

  • diameter (float > 0) – the diameter of the hole

  • cskDiameter (float) – the diameter of the countersink, must be greater than hole diameter

  • cskAngle (float > 0) – angle of the countersink, in degrees ( 82 is common )

  • depth (float > 0 or None to drill thru the entire part.) – the depth of the hole

  • clean (bool) – call clean() afterwards to have a clean shape

Return type

T

The surface of the hole is at the current workplane.

One hole is created for each item on the stack. A very common use case is to use a construction rectangle to define the centers of a set of holes, like so:

s = (
    Workplane()
    .box(2, 4, 0.5)
    .faces(">Z")
    .workplane()
    .rect(1.5, 3.5, forConstruction=True)
    .vertices()
    .cskHole(0.125, 0.25, 82, depth=None)
)

This sample creates a plate with a set of holes at the corners.

Plugin Note: this is one example of the power of plugins. CounterSunk holes are quite time consuming to create, but are quite easily defined by users.

see cboreHole() to make counterbores instead of countersinks

cut(toCut: Union[Workplane, Solid, Compound], clean: bool = True, tol: Optional[float] = None) → T[source]

Cuts the provided solid from the current solid, IE, perform a solid subtraction.

Parameters

  • self (T) –

  • toCut (Union[Workplane, Solid, Compound]) – a solid object, or a Workplane object having a solid

  • clean (bool) – call clean() afterwards to have a clean shape

  • tol (Optional[float]) – tolerance value for fuzzy bool operation mode (default None)

Raises

ValueError – if there is no solid to subtract from in the chain

Returns

a Workplane object with the resulting object selected

Return type

T

cutBlind(until: Union[float, Literal['next', 'last'], Face], clean: bool = True, both: bool = False, taper: Optional[float] = None) → T[source]

Use all un-extruded wires in the parent chain to create a prismatic cut from existing solid.

Specify either a distance value, or one of “next”, “last” to indicate a face to cut to.

Similar to extrude, except that a solid in the parent chain is required to remove material from. cutBlind always removes material from a part.

Parameters

  • self (T) –

  • until (Union[float, Literal['next', 'last'], Face]) – The distance to cut to, normal to the workplane plane. When a negative float is passed the cut extends this far in the opposite direction to the normal of the plane (i.e in the solid). The string “next” cuts until the next face orthogonal to the wire normal. “last” cuts to the last face. If an object of type Face is passed, then the cut will extend until this face.

  • clean (bool) – call clean() afterwards to have a clean shape

  • both (bool) – cut in both directions symmetrically

  • taper (Optional[float]) – angle for optional tapered extrusion

Raises

ValueError – if there is no solid to subtract from in the chain

Returns

a CQ object with the resulting object selected

Return type

T

see cutThruAll() to cut material from the entire part

cutEach(fcn: Callable[[Location], Shape], useLocalCoords: bool = False, clean: bool = True) → T[source]

Evaluates the provided function at each point on the stack (ie, eachpoint) and then cuts the result from the context solid.

Parameters

  • self (T) –

  • fcn (Callable[[Location], Shape]) – a function suitable for use in the eachpoint method: ie, that accepts a vector

  • useLocalCoords (bool) – same as for eachpoint()

  • clean (bool) – call clean() afterwards to have a clean shape

Raises

ValueError – if no solids or compounds are found in the stack or parent chain

Returns

a CQ object that contains the resulting solid

Return type

T

cutThruAll(clean: bool = True, taper: float = 0) → T[source]

Use all un-extruded wires in the parent chain to create a prismatic cut from existing solid. Cuts through all material in both normal directions of workplane.

Similar to extrude, except that a solid in the parent chain is required to remove material from. cutThruAll always removes material from a part.

Parameters

  • self (T) –

  • clean (bool) – call clean() afterwards to have a clean shape

  • taper (float) –

Raises

  • ValueError – if there is no solid to subtract from in the chain

  • ValueError – if there are no pending wires to cut with

Returns

a CQ object with the resulting object selected

Return type

T

see cutBlind() to cut material to a limited depth

cylinder(height: float, radius: float, direct: ~cadquery.occ_impl.geom.Vector = Vector: (0.0, 0.0, 1.0), angle: float = 360, centered: ~typing.Union[bool, ~typing.Tuple[bool, bool, bool]] = True, combine: ~typing.Union[bool, ~typing.Literal['cut', 'a', 's']] = True, clean: bool = True) → T[source]

Returns a cylinder with the specified radius and height for each point on the stack

Parameters

  • self (T) –

  • height (float) – The height of the cylinder

  • radius (float) – The radius of the cylinder

  • direct (A three-tuple) – The direction axis for the creation of the cylinder

  • angle (float > 0) – The angle to sweep the cylinder arc through

  • centered (Union[bool, Tuple[bool, bool, bool]]) – If True, the cylinder will be centered around the reference point. If False, the corner of a bounding box around the cylinder will be on the reference point and it will extend in the positive x, y and z directions. Can also use a 3-tuple to specify centering along each axis.

  • combine (true to combine shapes, false otherwise) – Whether the results should be combined with other solids on the stack (and each other)

  • clean (bool) – call clean() afterwards to have a clean shape

Returns

A cylinder object for each point on the stack

Return type

T

One cylinder is created for each item on the current stack. If no items are on the stack, one cylinder is created using the current workplane center.

If combine is true, the result will be a single object on the stack. If a solid was found in the chain, the result is that solid with all cylinders produced fused onto it otherwise, the result is the combination of all the produced cylinders.

If combine is false, the result will be a list of the cylinders produced.

each(callback: Callable[[Union[Vector, Location, Shape, Sketch]], Shape], useLocalCoordinates: bool = False, combine: Union[bool, Literal['cut', 'a', 's']] = True, clean: bool = True) → T[source]

Runs the provided function on each value in the stack, and collects the return values into a new CQ object.

Special note: a newly created workplane always has its center point as its only stack item

Parameters

  • self (T) –

  • callBackFunction – the function to call for each item on the current stack.

  • useLocalCoordinates (bool) – should values be converted from local coordinates first?

  • combine (Union[bool, Literal['cut', 'a', 's']]) – True or “a” to combine the resulting solid with parent solids if found, “cut” or “s” to remove the resulting solid from the parent solids if found. False to keep the resulting solid separated from the parent solids.

  • clean (bool) – call clean() afterwards to have a clean shape

  • callback (Callable[[Union[Vector, Location, Shape, Sketch]], Shape]) –

Return type

T

The callback function must accept one argument, which is the item on the stack, and return one object, which is collected. If the function returns None, nothing is added to the stack. The object passed into the callBackFunction is potentially transformed to local coordinates, if useLocalCoordinates is true

useLocalCoordinates is very useful for plugin developers.

If false, the callback function is assumed to be working in global coordinates. Objects created are added as-is, and objects passed into the function are sent in using global coordinates

If true, the calling function is assumed to be working in local coordinates. Objects are transformed to local coordinates before they are passed into the callback method, and result objects are transformed to global coordinates after they are returned.

This allows plugin developers to create objects in local coordinates, without worrying about the fact that the working plane is different than the global coordinate system.

TODO: wrapper object for Wire will clean up forConstruction flag everywhere

eachpoint(arg: Union[Shape, Workplane, Callable[[Location], Shape]], useLocalCoordinates: bool = False, combine: Union[bool, Literal['cut', 'a', 's']] = False, clean: bool = True) → T[source]

Same as each(), except arg is translated by the positions on the stack. If arg is a callback function, then the function is called for each point on the stack, and the resulting shape is used. :return: CadQuery object which contains a list of vectors (points ) on its stack.

Parameters

  • self (T) –

  • useLocalCoordinates (bool) – should points be in local or global coordinates

  • combine (Union[bool, Literal['cut', 'a', 's']]) – True or “a” to combine the resulting solid with parent solids if found, “cut” or “s” to remove the resulting solid from the parent solids if found. False to keep the resulting solid separated from the parent solids.

  • clean (bool) – call clean() afterwards to have a clean shape

  • arg (Union[Shape, Workplane, Callable[[Location], Shape]]) –

Return type

T

The resulting object has a point on the stack for each object on the original stack. Vertices and points remain a point. Faces, Wires, Solids, Edges, and Shells are converted to a point by using their center of mass.

If the stack has zero length, a single point is returned, which is the center of the current workplane/coordinate system

edges(selector: Optional[Union[str, Selector]] = None, tag: Optional[str] = None) → T[source]

Select the edges of objects on the stack, optionally filtering the selection. If there are multiple objects on the stack, the edges of all objects are collected and a list of all the distinct edges is returned.

Parameters

  • self (T) –

  • selector (Optional[Union[str, Selector]]) – optional Selector object, or string selector expression (see StringSyntaxSelector)

  • tag (Optional[str]) – if set, search the tagged object instead of self

Returns

a CQ object whose stack contains all of the distinct edges of all objects on the current stack, filtered by the provided selector.

Return type

T

If there are no edges for any objects on the current stack, an empty CQ object is returned

The typical use is to select the edges of a single object on the stack. For example:

Workplane().box(1, 1, 1).faces("+Z").edges().size()

returns 4, because the topmost face of a cube will contain four edges. Similarly:

Workplane().box(1, 1, 1).edges().size()

returns 12, because a cube has a total of 12 edges, And:

Workplane().box(1, 1, 1).edges("|Z").size()

returns 4, because a cube has 4 edges parallel to the z direction

ellipse(x_radius: float, y_radius: float, rotation_angle: float = 0.0, forConstruction: bool = False) → T[source]

Make an ellipse for each item on the stack.

Parameters

  • self (T) –

  • x_radius (float) – x radius of the ellipse (x-axis of plane the ellipse should lie in)

  • y_radius (float) – y radius of the ellipse (y-axis of plane the ellipse should lie in)

  • rotation_angle (float) – angle to rotate the ellipse

  • forConstruction (true if the wires are for reference, false if they are creating part geometry) – should the new wires be reference geometry only?

Returns

a new CQ object with the created wires on the stack

Return type

T

NOTE Due to a bug in opencascade (https://tracker.dev.opencascade.org/view.php?id=31290) the center of mass (equals center for next shape) is shifted. To create concentric ellipses use:

Workplane("XY").center(10, 20).ellipse(100, 10).center(0, 0).ellipse(50, 5)
ellipseArc(x_radius: float, y_radius: float, angle1: float = 360, angle2: float = 360, rotation_angle: float = 0.0, sense: Literal[- 1, 1] = 1, forConstruction: bool = False, startAtCurrent: bool = True, makeWire: bool = False) → T[source]

Draw an elliptical arc with x and y radiuses either with start point at current point or or current point being the center of the arc

Parameters

  • self (T) –

  • x_radius (float) – x radius of the ellipse (along the x-axis of plane the ellipse should lie in)

  • y_radius (float) – y radius of the ellipse (along the y-axis of plane the ellipse should lie in)

  • angle1 (float) – start angle of arc

  • angle2 (float) – end angle of arc (angle2 == angle1 return closed ellipse = default)

  • rotation_angle (float) – angle to rotate the created ellipse / arc

  • sense (Literal[-1, 1]) – clockwise (-1) or counter clockwise (1)

  • startAtCurrent (bool) – True: start point of arc is moved to current point; False: center of arc is on current point

  • makeWire (bool) – convert the resulting arc edge to a wire

  • forConstruction (bool) –

Return type

T

end(n: int = 1) → Workplane[source]

Return the nth parent of this CQ element

Parameters

n (int) – number of ancestor to return (default: 1)

Return type

a CQ object

Raises

ValueError if there are no more parents in the chain.

For example:

CQ(obj).faces("+Z").vertices().end()

will return the same as:

CQ(obj).faces("+Z")
export(fname: str, tolerance: float = 0.1, angularTolerance: float = 0.1, opt: Optional[Dict[str, Any]] = None) → T[source]

Export Workplane to file.

Parameters

  • self (T) –

  • path – Filename.

  • tolerance (float) – the deflection tolerance, in model units. Default 0.1.

  • angularTolerance (float) – the angular tolerance, in radians. Default 0.1.

  • opt (Optional[Dict[str, Any]]) – additional options passed to the specific exporter. Default None.

  • fname (str) –

Returns

Self.

Return type

T

exportSvg(fileName: str) → None[source]

Exports the first item on the stack as an SVG file

For testing purposes mainly.

Parameters

fileName (str) – the filename to export, absolute path to the file

Return type

None

extrude(until: Union[float, Literal['next', 'last'], Face], combine: Union[bool, Literal['cut', 'a', 's']] = True, clean: bool = True, both: bool = False, taper: Optional[float] = None) → T[source]

Use all un-extruded wires in the parent chain to create a prismatic solid.

Parameters

  • self (T) –

  • until (Union[float, Literal['next', 'last'], Face]) – The distance to extrude, normal to the workplane plane. When a float is passed, the extrusion extends this far and a negative value is in the opposite direction to the normal of the plane. The string “next” extrudes until the next face orthogonal to the wire normal. “last” extrudes to the last face. If a object of type Face is passed then the extrusion will extend until this face. Note that the Workplane must contain a Solid for extruding to a given face.

  • combine (Union[bool, Literal['cut', 'a', 's']]) – True or “a” to combine the resulting solid with parent solids if found, “cut” or “s” to remove the resulting solid from the parent solids if found. False to keep the resulting solid separated from the parent solids.

  • clean (bool) – call clean() afterwards to have a clean shape

  • both (bool) – extrude in both directions symmetrically

  • taper (Optional[float]) – angle for optional tapered extrusion

Returns

a CQ object with the resulting solid selected.

Return type

T

The returned object is always a CQ object, and depends on whether combine is True, and whether a context solid is already defined:

  • if combine is False, the new value is pushed onto the stack. Note that when extruding

    until a specified face, combine can not be False

  • if combine is true, the value is combined with the context solid if it exists,

    and the resulting solid becomes the new context solid.

faces(selector: Optional[Union[str, Selector]] = None, tag: Optional[str] = None) → T[source]

Select the faces of objects on the stack, optionally filtering the selection. If there are multiple objects on the stack, the faces of all objects are collected and a list of all the distinct faces is returned.

Parameters

  • self (T) –

  • selector (Optional[Union[str, Selector]]) – optional Selector object, or string selector expression (see StringSyntaxSelector)

  • tag (Optional[str]) – if set, search the tagged object instead of self

Returns

a CQ object whose stack contains all of the distinct faces of all objects on the current stack, filtered by the provided selector.

Return type

T

If there are no faces for any objects on the current stack, an empty CQ object is returned.

The typical use is to select the faces of a single object on the stack. For example:

Workplane().box(1, 1, 1).faces("+Z").size()

returns 1, because a cube has one face with a normal in the +Z direction. Similarly:

Workplane().box(1, 1, 1).faces().size()

returns 6, because a cube has a total of 6 faces, And:

Workplane().box(1, 1, 1).faces("|Z").size()

returns 2, because a cube has 2 faces having normals parallel to the z direction

fillet(radius: float) → T[source]

Fillets a solid on the selected edges.

The edges on the stack are filleted. The solid to which the edges belong must be in the parent chain of the selected edges.

Parameters

  • self (T) –

  • radius (float) – the radius of the fillet, must be > zero

Raises

  • ValueError – if at least one edge is not selected

  • ValueError – if the solid containing the edge is not in the chain

Returns

CQ object with the resulting solid selected.

Return type

T

This example will create a unit cube, with the top edges filleted:

s = Workplane().box(1, 1, 1).faces("+Z").edges().fillet(0.1)
filter(f: Callable[[Union[Vector, Location, Shape, Sketch]], bool]) → T[source]

Filter items using a boolean predicate.

Parameters
Returns

Workplane object with filtered items.

Return type

T

findFace(searchStack: bool = True, searchParents: bool = True) → Face[source]

Finds the first face object in the chain, searching from the current node backwards through parents until one is found.

Parameters

  • searchStack (bool) – should objects on the stack be searched first.

  • searchParents (bool) – should parents be searched?

Returns

A face or None if no face is found.

Return type

Face

findSolid(searchStack: bool = True, searchParents: bool = True) → Union[Solid, Compound][source]

Finds the first solid object in the chain, searching from the current node backwards through parents until one is found.

Parameters

  • searchStack (bool) – should objects on the stack be searched first?

  • searchParents (bool) – should parents be searched?

Raises

ValueError – if no solid is found

Return type

Union[Solid, Compound]

This function is very important for chains that are modifying a single parent object, most often a solid.

Most of the time, a chain defines or selects a solid, and then modifies it using workplanes or other operations.

Plugin Developers should make use of this method to find the solid that should be modified, if the plugin implements a unary operation, or if the operation will automatically merge its results with an object already on the stack.

first() → T[source]

Return the first item on the stack

Returns

the first item on the stack.

Return type

a CQ object

Parameters

self (T) –

hLine(distance: float, forConstruction: bool = False) → T[source]

Make a horizontal line from the current point the provided distance

Parameters

  • self (T) –

  • distance (float) –

    1. distance from current point

  • forConstruction (bool) –

Returns

the Workplane object with the current point at the end of the new line

Return type

T

hLineTo(xCoord: float, forConstruction: bool = False) → T[source]

Make a horizontal line from the current point to the provided x coordinate.

Useful if it is more convenient to specify the end location rather than distance, as in hLine()

Parameters

  • self (T) –

  • xCoord (float) – x coordinate for the end of the line

  • forConstruction (bool) –

Returns

the Workplane object with the current point at the end of the new line

Return type

T

hole(diameter: float, depth: Optional[float] = None, clean: bool = True) → T[source]

Makes a hole for each item on the stack.

Parameters

  • self (T) –

  • diameter (float) – the diameter of the hole

  • depth (float > 0 or None to drill thru the entire part.) – the depth of the hole

  • clean (bool) – call clean() afterwards to have a clean shape

Return type

T

The surface of the hole is at the current workplane.

One hole is created for each item on the stack. A very common use case is to use a construction rectangle to define the centers of a set of holes, like so:

s = (
    Workplane()
    .box(2, 4, 0.5)
    .faces(">Z")
    .workplane()
    .rect(1.5, 3.5, forConstruction=True)
    .vertices()
    .hole(0.125, 82)
)

This sample creates a plate with a set of holes at the corners.

Plugin Note: this is one example of the power of plugins. CounterSunk holes are quite time consuming to create, but are quite easily defined by users.

see cboreHole() and cskHole() to make counterbores or countersinks

interpPlate(surf_edges: Union[Sequence[Union[Tuple[float, float], Tuple[float, float, float], Vector]], Sequence[Union[Edge, Wire]], Workplane], surf_pts: Sequence[Union[Tuple[float, float], Tuple[float, float, float], Vector]] = [], thickness: float = 0, combine: Union[bool, Literal['cut', 'a', 's']] = False, clean: bool = True, degree: int = 3, nbPtsOnCur: int = 15, nbIter: int = 2, anisotropy: bool = False, tol2d: float = 1e-05, tol3d: float = 0.0001, tolAng: float = 0.01, tolCurv: float = 0.1, maxDeg: int = 8, maxSegments: int = 9) → T[source]

Returns a plate surface that is ‘thickness’ thick, enclosed by ‘surf_edge_pts’ points, and going through ‘surf_pts’ points. Using pushPoints directly with interpPlate and combine=True, can be very resource intensive depending on the complexity of the shape. In this case set combine=False.

Parameters

  • self (T) –

  • surf_edges (Union[Sequence[Union[Tuple[float, float], Tuple[float, float, float], Vector]], Sequence[Union[Edge, Wire]], Workplane]) – list of [x,y,z] ordered coordinates or list of ordered or unordered edges, wires

  • surf_pts (Sequence[Union[Tuple[float, float], Tuple[float, float, float], Vector]]) – list of points (uses only edges if [])

  • thickness (float) – value may be negative or positive depending on thickening direction (2D surface if 0)

  • combine (Union[bool, Literal['cut', 'a', 's']]) – should the results be combined with other solids on the stack (and each other)?

  • clean (bool) – call clean() afterwards to have a clean shape

  • degree (int) – >= 2

  • nbPtsOnCur (int) – number of points on curve >= 15

  • nbIter (int) – number of iterations >= 2

  • anisotropy (bool) – = bool Anisotropy

  • tol2d (float) – 2D tolerance

  • tol3d (float) – 3D tolerance

  • tolAng (float) – angular tolerance

  • tolCurv (float) – tolerance for curvature

  • maxDeg (int) – highest polynomial degree >= 2

  • maxSegments (int) – greatest number of segments >= 2

Return type

T

intersect(toIntersect: Union[Workplane, Solid,