# Introductory Examples

The examples on this page can help you learn how to build objects with build123d, and are intended as a general overview of build123d.

They are organized from simple to complex, so working through them in order is the best way to absorb them.

Note

Some important lines are omitted below to save space, so you will most likely need to add 1 & 2 to the provided code below for them to work:

`from build123d import *`

If you are using build123d

builder modeoralgebra mode,

in

ocp_vscodesimply use e.g.`show(ex15)`

to the end of your design to view parts, sketches and curves.`show_all()`

can be used to automatically show all objects with their variable names as labels.in

CQ-editoradd e.g.`show_object(ex15.part)`

,`show_object(ex15.sketch)`

or`show_object(ex15.line)`

to the end of your design to view parts, sketches or lines.If you want to save your resulting object as an STL from

builder mode, you can use e.g.`export_stl(ex15.part, "file.stl")`

.If you want to save your resulting object as an STL from

algebra mode, you can use e.g.`export_stl(ex15, "file.stl")`

build123d also supports exporting to multiple other file formats including STEP, see here for further information: Import/Export Formats

## 1. Simple Rectangular Plate

Just about the simplest possible example, a rectangular `Box`

.

**Builder mode**length, width, thickness = 80.0, 60.0, 10.0 with BuildPart() as ex1: Box(length, width, thickness)

**Algebra mode**length, width, thickness = 80.0, 60.0, 10.0 ex1 = Box(length, width, thickness)

## 3. An extruded prismatic solid

Build a prismatic solid using extrusion.

**Builder mode**This time we can first create a 2D

`BuildSketch`

adding a`Circle`

and a subtracted`Rectangle``

and then use`BuildPart`

’s`extrude()`

feature.length, width, thickness = 80.0, 60.0, 10.0 with BuildPart() as ex3: with BuildSketch() as ex3_sk: Circle(width) Rectangle(length / 2, width / 2, mode=Mode.SUBTRACT) extrude(amount=2 * thickness)

**Algebra mode**

## 4. Building Profiles using lines and arcs

Sometimes you need to build complex profiles using lines and arcs. This example builds a prismatic solid from 2D operations. It is not necessary to create variables for the line segments, but it will be useful in a later example.

**Builder mode**`BuildSketch`

operates on closed Faces, and the operation`make_face()`

is used to convert the pending line segments from`BuildLine`

into a closed Face.length, width, thickness = 80.0, 60.0, 10.0 with BuildPart() as ex4: with BuildSketch() as ex4_sk: with BuildLine() as ex4_ln: l1 = Line((0, 0), (length, 0)) l2 = Line((length, 0), (length, width)) l3 = ThreePointArc((length, width), (width, width * 1.5), (0.0, width)) l4 = Line((0.0, width), (0, 0)) make_face() extrude(amount=thickness)

**Algebra mode**We start with an empty

`Curve`

and add lines to it (note that`Curve() + [line1, line2, line3]`

is much more efficient than`line1 + line2 + line3`

, see Performance considerations in algebra mode). The operation`make_face()`

is used to convert the line segments into a Face.length, width, thickness = 80.0, 60.0, 10.0 lines = Curve() + [ Line((0, 0), (length, 0)), Line((length, 0), (length, width)), ThreePointArc((length, width), (width, width * 1.5), (0.0, width)), Line((0.0, width), (0, 0)), ] sk4 = make_face(lines) ex4 = extrude(sk4, thickness)

Note that to build a closed face it requires line segments that form a closed shape.

## 5. Moving the current working point

**Builder mode**Using

`Locations`

we can place one (or multiple) objects at one (or multiple) places.a, b, c, d = 90, 45, 15, 7.5 with BuildPart() as ex5: with BuildSketch() as ex5_sk: Circle(a) with Locations((b, 0.0)): Rectangle(c, c, mode=Mode.SUBTRACT) with Locations((0, b)): Circle(d, mode=Mode.SUBTRACT) extrude(amount=c)

**Algebra mode**Using the pattern

`Pos(x, y, z=0) * obj`

(with`geometry.Pos`

) we can move an object to the provided position. Using`Rot(x_angle, y_angle, z_angle) * obj`

(with`geometry.Rot`

) would rotate the object.a, b, c, d = 90, 45, 15, 7.5 sk5 = Circle(a) - Pos(b, 0.0) * Rectangle(c, c) - Pos(0.0, b) * Circle(d) ex5 = extrude(sk5, c)

## 6. Using Point Lists

Sometimes you need to create a number of features at various
`Locations`

.

**Builder mode**You can use a list of points to construct multiple objects at once.

a, b, c = 80, 60, 10 with BuildPart() as ex6: with BuildSketch() as ex6_sk: Circle(a) with Locations((b, 0), (0, b), (-b, 0), (0, -b)): Circle(c, mode=Mode.SUBTRACT) extrude(amount=c)

**Algebra mode**You can use loops to iterate over these Locations or list comprehensions as in the example.

The algebra operations are vectorized, which means

`obj - [obj1, obj2, obj3]`

is short for`obj - obj1 - obj2 - ob3`

(and more efficient, see Performance considerations in algebra mode).a, b, c = 80, 60, 10 sk6 = [loc * Circle(c) for loc in Locations((b, 0), (0, b), (-b, 0), (0, -b))] ex6 = extrude(Circle(a) - sk6, c)

## 7. Polygons

**Builder mode**You can create

`RegularPolygon`

for each stack point if you would like.a, b, c = 60, 80, 5 with BuildPart() as ex7: with BuildSketch() as ex7_sk: Rectangle(a, b) with Locations((0, 3 * c), (0, -3 * c)): RegularPolygon(radius=2 * c, side_count=6, mode=Mode.SUBTRACT) extrude(amount=c)

**Algebra mode**You can apply locations to

`RegularPolygon`

instances for each location via loops or list comprehensions.a, b, c = 60, 80, 5 polygons = [ loc * RegularPolygon(radius=2 * c, side_count=6) for loc in Locations((0, 3 * c), (0, -3 * c)) ] sk7 = Rectangle(a, b) - polygons ex7 = extrude(sk7, amount=c)

## 8. Polylines

`Polyline`

allows creating a shape from a large number
of chained points connected by lines. This example uses a polyline to create
one half of an i-beam shape, which is `mirror()`

ed to
create the final profile.

**Builder mode**(L, H, W, t) = (100.0, 20.0, 20.0, 1.0) pts = [ (0, H / 2.0), (W / 2.0, H / 2.0), (W / 2.0, (H / 2.0 - t)), (t / 2.0, (H / 2.0 - t)), (t / 2.0, (t - H / 2.0)), (W / 2.0, (t - H / 2.0)), (W / 2.0, H / -2.0), (0, H / -2.0), ] with BuildPart() as ex8: with BuildSketch(Plane.YZ) as ex8_sk: with BuildLine() as ex8_ln: Polyline(pts) mirror(ex8_ln.line, about=Plane.YZ) make_face() extrude(amount=L)

**Algebra mode**(L, H, W, t) = (100.0, 20.0, 20.0, 1.0) pts = [ (0, H / 2.0), (W / 2.0, H / 2.0), (W / 2.0, (H / 2.0 - t)), (t / 2.0, (H / 2.0 - t)), (t / 2.0, (t - H / 2.0)), (W / 2.0, (t - H / 2.0)), (W / 2.0, H / -2.0), (0, H / -2.0), ] ln = Polyline(pts) ln += mirror(ln, Plane.YZ) sk8 = make_face(Plane.YZ * ln) ex8 = extrude(sk8, -L).clean()

## 9. Selectors, Fillets, and Chamfers

This example introduces multiple useful and important concepts. Firstly `chamfer()`

and `fillet()`

can be used to “bevel” and “round” edges respectively. Secondly,
these two methods require an edge or a list of edges to operate on. To select all
edges, you could simply pass in `ex9.edges()`

.

**Builder mode**length, width, thickness = 80.0, 60.0, 10.0 with BuildPart() as ex9: Box(length, width, thickness) chamfer(ex9.edges().group_by(Axis.Z)[-1], length=4) fillet(ex9.edges().filter_by(Axis.Z), radius=5)

**Algebra mode**length, width, thickness = 80.0, 60.0, 10.0 ex9 = Part() + Box(length, width, thickness) ex9 = chamfer(ex9.edges().group_by(Axis.Z)[-1], length=4) ex9 = fillet(ex9.edges().filter_by(Axis.Z), radius=5)

Note that `group_by()`

`(Axis.Z)`

returns a list of lists of edges that is grouped by
their z-position. In this case we want to use the `[-1]`

group which, by convention, will
be the highest z-dimension group.

## 10. Select Last and Hole

**Builder mode**Using

`Select`

`.LAST`

you can select the most recently modified edges. It is used to perform a`fillet()`

in this example. This example also makes use of`Hole`

which automatically cuts through the entire part.length, width, thickness = 80.0, 60.0, 10.0 with BuildPart() as ex10: Box(length, width, thickness) Hole(radius=width / 4) fillet(ex10.edges(Select.LAST).group_by(Axis.Z)[-1], radius=2)

**Algebra mode**Using the pattern

`snapshot = obj.edges()`

before and`last_edges = obj.edges() - snapshot`

after an operation allows to select the most recently modified edges (same for`faces`

,`vertices`

, …). It is used to perform a`fillet()`

in this example. This example also makes use of`Hole`

. Different to the*context mode*, you have to add the`depth`

of the whole.ex10 = Part() + Box(length, width, thickness) snapshot = ex10.edges() ex10 -= Hole(radius=width / 4, depth=thickness) last_edges = ex10.edges() - snapshot ex10 = fillet(last_edges.group_by(Axis.Z)[-1], 2)

## 11. Use a face as a plane for BuildSketch and introduce GridLocations

**Builder mode**`BuildSketch`

accepts a Plane or a Face, so in this case we locate the Sketch on the top of the part. Note that the face used as input to BuildSketch needs to be Planar or unpredictable behavior can result. Additionally`GridLocations`

can be used to create a grid of points that are simultaneously used to place 4 pentagons.Lastly,

`extrude()`

can be used with a negative amount and`Mode.SUBTRACT`

to cut these from the parent.length, width, thickness = 80.0, 60.0, 10.0 with BuildPart() as ex11: Box(length, width, thickness) chamfer(ex11.edges().group_by(Axis.Z)[-1], length=4) fillet(ex11.edges().filter_by(Axis.Z), radius=5) Hole(radius=width / 4) fillet(ex11.edges(Select.LAST).sort_by(Axis.Z)[-1], radius=2) with BuildSketch(ex11.faces().sort_by(Axis.Z)[-1]) as ex11_sk: with GridLocations(length / 2, width / 2, 2, 2): RegularPolygon(radius=5, side_count=5) extrude(amount=-thickness, mode=Mode.SUBTRACT)

**Algebra mode**The pattern

`plane * obj`

can be used to locate an object on a plane. Furthermore, the pattern`plane * location * obj`

first places the object on a plane and then moves it relative to plane according to`location`

.`GridLocations`

creates a grid of points that can be used in loops or list comprehensions as described earlier.Lastly,

`extrude()`

can be used with a negative amount and cut (`-`

) from the parent.length, width, thickness = 80.0, 60.0, 10.0 ex11 = Part() + Box(length, width, thickness) ex11 = chamfer(ex11.edges().group_by()[-1], 4) ex11 = fillet(ex11.edges().filter_by(Axis.Z), 5) last = ex11.edges() ex11 -= Hole(radius=width / 4, depth=thickness) ex11 = fillet((ex11.edges() - last).sort_by().last, 2) plane = Plane(ex11.faces().sort_by().last) polygons = Sketch() + [ plane * loc * RegularPolygon(radius=5, side_count=5) for loc in GridLocations(length / 2, width / 2, 2, 2) ] ex11 -= extrude(polygons, -thickness)

Note that the direction implied by positive or negative inputs to amount is relative to the
normal direction of the face or plane. As a result of this, unexpected behavior can occur
if the extrude direction and mode/operation (ADD / `+`

or SUBTRACT / `-`

) are not correctly set.

## 12. Defining an Edge with a Spline

This example defines a side using a spline curve through a collection of points. Useful when you have an edge that needs a complex profile.

**Builder mode**pts = [ (55, 30), (50, 35), (40, 30), (30, 20), (20, 25), (10, 20), (0, 20), ] with BuildPart() as ex12: with BuildSketch() as ex12_sk: with BuildLine() as ex12_ln: l1 = Spline(pts) l2 = Line((55, 30), (60, 0)) l3 = Line((60, 0), (0, 0)) l4 = Line((0, 0), (0, 20)) make_face() extrude(amount=10)

**Algebra mode**pts = [ (55, 30), (50, 35), (40, 30), (30, 20), (20, 25), (10, 20), (0, 20), ] l1 = Spline(pts) l2 = Line(l1 @ 0, (60, 0)) l3 = Line(l2 @ 1, (0, 0)) l4 = Line(l3 @ 1, l1 @ 1) sk12 = make_face([l1, l2, l3, l4]) ex12 = extrude(sk12, 10)

## 13. CounterBoreHoles, CounterSinkHoles and PolarLocations

Counter-sink and counter-bore holes are useful for creating recessed areas for fasteners.

**Builder mode**We use a face to establish a location for

`Locations`

.a, b = 40, 4 with BuildPart() as ex13: Cylinder(radius=50, height=10) with Locations(ex13.faces().sort_by(Axis.Z)[-1]): with PolarLocations(radius=a, count=4): CounterSinkHole(radius=b, counter_sink_radius=2 * b) with PolarLocations(radius=a, count=4, start_angle=45, angular_range=360): CounterBoreHole(radius=b, counter_bore_radius=2 * b, counter_bore_depth=b)

**Algebra mode**We use a face to establish a plane that is used later in the code for locating objects onto this plane.

a, b = 40, 4 ex13 = Cylinder(radius=50, height=10) plane = Plane(ex13.faces().sort_by().last) ex13 -= ( plane * PolarLocations(radius=a, count=4) * CounterSinkHole(radius=b, counter_sink_radius=2 * b, depth=10) ) ex13 -= ( plane * PolarLocations(radius=a, count=4, start_angle=45, angular_range=360) * CounterBoreHole( radius=b, counter_bore_radius=2 * b, depth=10, counter_bore_depth=b ) )

`PolarLocations`

creates a list of points that are radially distributed.

## 14. Position on a line with ‘@’, ‘%’ and introduce Sweep

build123d includes a feature for finding the position along a line segment. This
is normalized between 0 and 1 and can be accessed using the `position_at()`

(@) operator.
Similarly the `tangent_at()`

(%) operator returns the line direction at a given point.

These two features are very powerful for chaining line segments together without having to repeat dimensions again and again, which is error prone, time consuming, and more difficult to maintain. The pending faces must lie on the path, please see example 37 for a way to make this placement easier.

**Builder mode**The

`sweep()`

method takes any pending faces and sweeps them through the provided path (in this case the path is taken from the pending edges from`ex14_ln`

).`revolve()`

requires a single connected wire.a, b = 40, 20 with BuildPart() as ex14: with BuildLine() as ex14_ln: l1 = JernArc(start=(0, 0), tangent=(0, 1), radius=a, arc_size=180) l2 = JernArc(start=l1 @ 1, tangent=l1 % 1, radius=a, arc_size=-90) l3 = Line(l2 @ 1, l2 @ 1 + (-a, a)) with BuildSketch(Plane.XZ) as ex14_sk: Rectangle(b, b) sweep()

**Algebra mode**The

`sweep()`

method takes any faces and sweeps them through the provided path (in this case the path is taken from`ex14_ln`

).a, b = 40, 20 l1 = JernArc(start=(0, 0), tangent=(0, 1), radius=a, arc_size=180) l2 = JernArc(start=l1 @ 1, tangent=l1 % 1, radius=a, arc_size=-90) l3 = Line(l2 @ 1, l2 @ 1 + (-a, a)) ex14_ln = l1 + l2 + l3 sk14 = Plane.XZ * Rectangle(b, b) ex14 = sweep(sk14, path=ex14_ln)

It is also possible to use tuple or `Vector`

addition (and other vector math operations)
as seen in the `l3`

variable.

## 15. Mirroring Symmetric Geometry

Here mirror is used on the BuildLine to create a symmetric shape with fewer line segment commands. Additionally the ‘@’ operator is used to simplify the line segment commands.

`(l4 @ 1).Y`

is used to extract the y-component of the `l4 @ 1`

vector.

**Builder mode**a, b, c = 80, 40, 20 with BuildPart() as ex15: with BuildSketch() as ex15_sk: with BuildLine() as ex15_ln: l1 = Line((0, 0), (a, 0)) l2 = Line(l1 @ 1, l1 @ 1 + (0, b)) l3 = Line(l2 @ 1, l2 @ 1 + (-c, 0)) l4 = Line(l3 @ 1, l3 @ 1 + (0, -c)) l5 = Line(l4 @ 1, (0, (l4 @ 1).Y)) mirror(ex15_ln.line, about=Plane.YZ) make_face() extrude(amount=c)

**Algebra mode**Combine lines via the pattern

`Curve() + [l1, l2, l3, l4, l5]`

a, b, c = 80, 40, 20 l1 = Line((0, 0), (a, 0)) l2 = Line(l1 @ 1, l1 @ 1 + (0, b)) l3 = Line(l2 @ 1, l2 @ 1 + (-c, 0)) l4 = Line(l3 @ 1, l3 @ 1 + (0, -c)) l5 = Line(l4 @ 1, (0, (l4 @ 1).Y)) ln = Curve() + [l1, l2, l3, l4, l5] ln += mirror(ln, Plane.YZ) sk15 = make_face(ln) ex15 = extrude(sk15, c)

## 16. Mirroring 3D Objects

Mirror can also be used with BuildPart (and BuildSketch) to mirror 3D objects.
The `Plane.offset()`

method shifts the plane in the normal direction (positive or negative).

**Builder mode**length, width, thickness = 80.0, 60.0, 10.0 with BuildPart() as ex16_single: with BuildSketch(Plane.XZ) as ex16_sk: Rectangle(length, width) fillet(ex16_sk.vertices(), radius=length / 10) with GridLocations(x_spacing=length / 4, y_spacing=0, x_count=3, y_count=1): Circle(length / 12, mode=Mode.SUBTRACT) Rectangle(length, width, align=(Align.MIN, Align.MIN), mode=Mode.SUBTRACT) extrude(amount=length) with BuildPart() as ex16: add(ex16_single.part) mirror(ex16_single.part, about=Plane.XY.offset(width)) mirror(ex16_single.part, about=Plane.YX.offset(width)) mirror(ex16_single.part, about=Plane.YZ.offset(width)) mirror(ex16_single.part, about=Plane.YZ.offset(-width))

**Algebra mode**length, width, thickness = 80.0, 60.0, 10.0 sk16 = Rectangle(length, width) sk16 = fillet(sk16.vertices(), length / 10) circles = [loc * Circle(length / 12) for loc in GridLocations(length / 4, 0, 3, 1)] sk16 = sk16 - circles - Rectangle(length, width, align=(Align.MIN, Align.MIN)) ex16_single = extrude(Plane.XZ * sk16, length) planes = [ Plane.XY.offset(width), Plane.YX.offset(width), Plane.YZ.offset(width), Plane.YZ.offset(-width), ] objs = [mirror(ex16_single, plane) for plane in planes] ex16 = ex16_single + objs

## 17. Mirroring From Faces

Here we select the farthest face in the Y-direction and turn it into a `Plane`

using the
`Plane()`

class.

**Builder mode**a, b = 30, 20 with BuildPart() as ex17: with BuildSketch() as ex17_sk: RegularPolygon(radius=a, side_count=5) extrude(amount=b) mirror(ex17.part, about=Plane(ex17.faces().group_by(Axis.Y)[0][0]))

**Algebra mode**a, b = 30, 20 sk17 = RegularPolygon(radius=a, side_count=5) ex17 = extrude(sk17, amount=b) ex17 += mirror(ex17, Plane(ex17.faces().sort_by(Axis.Y).first))

## 18. Creating Workplanes on Faces

Here we start with an earlier example, select the top face, draw a rectangle and then use Extrude with a negative distance.

**Builder mode**We then use

`Mode.SUBTRACT`

to cut it out from the main body.length, width, thickness = 80.0, 60.0, 10.0 a, b = 4, 5 with BuildPart() as ex18: Box(length, width, thickness) chamfer(ex18.edges().group_by(Axis.Z)[-1], length=a) fillet(ex18.edges().filter_by(Axis.Z), radius=b) with BuildSketch(ex18.faces().sort_by(Axis.Z)[-1]): Rectangle(2 * b, 2 * b) extrude(amount=-thickness, mode=Mode.SUBTRACT)

**Algebra mode**We then use

`-=`

to cut it out from the main body.length, width, thickness = 80.0, 60.0, 10.0 a, b = 4, 5 ex18 = Part() + Box(length, width, thickness) ex18 = chamfer(ex18.edges().group_by()[-1], a) ex18 = fillet(ex18.edges().filter_by(Axis.Z), b) sk18 = Plane(ex18.faces().sort_by().first) * Rectangle(2 * b, 2 * b) ex18 -= extrude(sk18, -thickness)

## 19. Locating a workplane on a vertex

Here a face is selected and two different strategies are used to select vertices.
Firstly `vtx`

uses `group_by()`

and `Axis.X`

to select a particular vertex. The second strategy uses a custom
defined Axis `vtx2Axis`

that is pointing roughly in the direction of a vertex to select, and then `sort_by()`

this custom Axis.

**Builder mode**Then the X and Y positions of these vertices are selected and passed to

`Locations`

as center points for two circles that cut through the main part. Note that if you passed the variable`vtx`

directly to`Locations`

then the part would be offset from the workplane by the vertex z-position.length, thickness = 80.0, 10.0 with BuildPart() as ex19: with BuildSketch() as ex19_sk: RegularPolygon(radius=length / 2, side_count=7) extrude(amount=thickness) topf = ex19.faces().sort_by(Axis.Z)[-1] vtx = topf.vertices().group_by(Axis.X)[-1][0] vtx2Axis = Axis((0, 0, 0), (-1, -0.5, 0)) vtx2 = topf.vertices().sort_by(vtx2Axis)[-1] with BuildSketch(topf) as ex19_sk2: with Locations((vtx.X, vtx.Y), (vtx2.X, vtx2.Y)): Circle(radius=length / 8) extrude(amount=-thickness, mode=Mode.SUBTRACT)

**Algebra mode**Then the X and Y positions of these vertices are selected and used to move two circles that cut through the main part. Note that if you passed the variable

`vtx`

directly to`Pos`

then the part would be offset from the workplane by the vertex z-position.length, thickness = 80.0, 10.0 ex19_sk = RegularPolygon(radius=length / 2, side_count=7) ex19 = extrude(ex19_sk, thickness) topf = ex19.faces().sort_by().last vtx = topf.vertices().group_by(Axis.X)[-1][0] vtx2Axis = Axis((0, 0, 0), (-1, -0.5, 0)) vtx2 = topf.vertices().sort_by(vtx2Axis)[-1] ex19_sk2 = Circle(radius=length / 8) ex19_sk2 = Pos(vtx.X, vtx.Y) * ex19_sk2 + Pos(vtx2.X, vtx2.Y) * ex19_sk2 ex19 -= extrude(ex19_sk2, thickness)

## 20. Offset Sketch Workplane

The `plane`

variable is set to be coincident with the farthest face in the
negative x-direction. The resulting Plane is offset from the original position.

**Builder mode**length, width, thickness = 80.0, 60.0, 10.0 with BuildPart() as ex20: Box(length, width, thickness) plane = Plane(ex20.faces().group_by(Axis.X)[0][0]) with BuildSketch(plane.offset(2 * thickness)): Circle(width / 3) extrude(amount=width)

**Algebra mode**length, width, thickness = 80.0, 60.0, 10.0 ex20 = Box(length, width, thickness) plane = Plane(ex20.faces().sort_by(Axis.X).first).offset(2 * thickness) sk20 = plane * Circle(width / 3) ex20 += extrude(sk20, width)

## 21. Create a Workplanes in the center of another shape

One cylinder is created, and then the origin and z_dir of that part are used to create a new Plane for positioning another cylinder perpendicular and halfway along the first.

**Builder mode**width, length = 10.0, 60.0 with BuildPart() as ex21: with BuildSketch() as ex21_sk: Circle(width / 2) extrude(amount=length) with BuildSketch(Plane(origin=ex21.part.center(), z_dir=(-1, 0, 0))): Circle(width / 2) extrude(amount=length)

**Algebra mode**width, length = 10.0, 60.0 ex21 = extrude(Circle(width / 2), length) plane = Plane(origin=ex21.center(), z_dir=(-1, 0, 0)) ex21 += plane * extrude(Circle(width / 2), length)

## 22. Rotated Workplanes

It is also possible to create a rotated workplane, building upon some of the concepts in an earlier example.

**Builder mode**Use the

`rotated()`

method to rotate the workplane.length, width, thickness = 80.0, 60.0, 10.0 with BuildPart() as ex22: Box(length, width, thickness) pln = Plane(ex22.faces().group_by(Axis.Z)[0][0]).rotated((0, -50, 0)) with BuildSketch(pln) as ex22_sk: with GridLocations(length / 4, width / 4, 2, 2): Circle(thickness / 4) extrude(amount=-100, both=True, mode=Mode.SUBTRACT)

**Algebra mode**Use the operator

`*`

to relocate the plane (post-multiplication!).length, width, thickness = 80.0, 60.0, 10.0 ex22 = Box(length, width, thickness) plane = Plane((ex22.faces().group_by(Axis.Z)[0])[0]) * Rot(0, 50, 0) holes = Sketch() + [ plane * loc * Circle(thickness / 4) for loc in GridLocations(length / 4, width / 4, 2, 2) ] ex22 -= extrude(holes, -100, both=True)

`GridLocations`

places 4 Circles on 4 points on this rotated workplane, and then the Circles are
extruded in the “both” (positive and negative) normal direction.

## 23. Revolve

Here we build a sketch with a `Polyline`

,
`Line`

, and a `Circle`

. It is
absolutely critical that the sketch is only on one side of the axis of rotation
before Revolve is called. To that end, `split`

is used with `Plane.ZY`

to keep
only one side of the Sketch.

It is highly recommended to view your sketch before you attempt to call revolve.

**Builder mode**pts = [ (-25, 35), (-25, 0), (-20, 0), (-20, 5), (-15, 10), (-15, 35), ] with BuildPart() as ex23: with BuildSketch(Plane.XZ) as ex23_sk: with BuildLine() as ex23_ln: l1 = Polyline(pts) l2 = Line(l1 @ 1, l1 @ 0) make_face() with Locations((0, 35)): Circle(25) split(bisect_by=Plane.ZY) revolve(axis=Axis.Z)

**Algebra mode**pts = [ (-25, 35), (-25, 0), (-20, 0), (-20, 5), (-15, 10), (-15, 35), ] l1 = Polyline(pts) l2 = Line(l1 @ 1, l1 @ 0) sk23 = make_face([l1, l2]) sk23 += Pos(0, 35) * Circle(25) sk23 = Plane.XZ * split(sk23, bisect_by=Plane.ZY) ex23 = revolve(sk23, Axis.Z)

## 24. Loft

Loft is a very powerful tool that can be used to join dissimilar shapes. In this case we make a
conical-like shape from a circle and a rectangle that is offset vertically. In this case
`loft()`

automatically takes the pending faces that were added by the two BuildSketches.
Loft can behave unexpectedly when the input faces are not parallel to each other.

**Builder mode**length, width, thickness = 80.0, 60.0, 10.0 with BuildPart() as ex24: Box(length, length, thickness) with BuildSketch(ex24.faces().group_by(Axis.Z)[0][0]) as ex24_sk: Circle(length / 3) with BuildSketch(ex24_sk.faces()[0].offset(length / 2)) as ex24_sk2: Rectangle(length / 6, width / 6) loft()

**Algebra mode**length, width, thickness = 80.0, 60.0, 10.0 ex24 = Box(length, length, thickness) plane = Plane(ex24.faces().sort_by().last) faces = Sketch() + [ plane * Circle(length / 3), plane.offset(length / 2) * Rectangle(length / 6, width / 6), ] ex24 += loft(faces)

## 25. Offset Sketch

**Builder mode**BuildSketch faces can be transformed with a 2D

`offset()`

.rad, offs = 50, 10 with BuildPart() as ex25: with BuildSketch() as ex25_sk1: RegularPolygon(radius=rad, side_count=5) with BuildSketch(Plane.XY.offset(15)) as ex25_sk2: RegularPolygon(radius=rad, side_count=5) offset(amount=offs) with BuildSketch(Plane.XY.offset(30)) as ex25_sk3: RegularPolygon(radius=rad, side_count=5) offset(amount=offs, kind=Kind.INTERSECTION) extrude(amount=1)

**Algebra mode**Sketch faces can be transformed with a 2D

`offset()`

.rad, offs = 50, 10 sk25_1 = RegularPolygon(radius=rad, side_count=5) sk25_2 = Plane.XY.offset(15) * RegularPolygon(radius=rad, side_count=5) sk25_2 = offset(sk25_2, offs) sk25_3 = Plane.XY.offset(30) * RegularPolygon(radius=rad, side_count=5) sk25_3 = offset(sk25_3, offs, kind=Kind.INTERSECTION) sk25 = Sketch() + [sk25_1, sk25_2, sk25_3] ex25 = extrude(sk25, 1)

They can be offset inwards or outwards, and with different techniques for extending the
corners (see `Kind`

in the Offset docs).

## 26. Offset Part To Create Thin features

Parts can also be transformed using an offset, but in this case with
a 3D `offset()`

. Also commonly known as a shell, this allows creating thin walls
using very few operations. This can also be offset inwards or outwards. Faces can be selected to be
“deleted” using the `openings`

parameter of `offset()`

.

Note that self intersecting edges and/or faces can break both 2D and 3D offsets.

**Builder mode**length, width, thickness, wall = 80.0, 60.0, 10.0, 2.0 with BuildPart() as ex26: Box(length, width, thickness) topf = ex26.faces().sort_by(Axis.Z)[-1] offset(amount=-wall, openings=topf)

**Algebra mode**length, width, thickness, wall = 80.0, 60.0, 10.0, 2.0 ex26 = Box(length, width, thickness) topf = ex26.faces().sort_by().last ex26 = offset(ex26, amount=-wall, openings=topf)

## 27. Splitting an Object

You can split an object using a plane, and retain either or both halves. In this case we select a face and offset half the width of the box.

**Builder mode**length, width, thickness = 80.0, 60.0, 10.0 with BuildPart() as ex27: Box(length, width, thickness) with BuildSketch(ex27.faces().sort_by(Axis.Z)[0]) as ex27_sk: Circle(width / 4) extrude(amount=-thickness, mode=Mode.SUBTRACT) split(bisect_by=Plane(ex27.faces().sort_by(Axis.Y)[-1]).offset(-width / 2))

**Algebra mode**length, width, thickness = 80.0, 60.0, 10.0 ex27 = Box(length, width, thickness) sk27 = Plane(ex27.faces().sort_by().first) * Circle(width / 4) ex27 -= extrude(sk27, -thickness) ex27 = split(ex27, Plane(ex27.faces().sort_by(Axis.Y).last).offset(-width / 2))

## 28. Locating features based on Faces

**Builder mode**We create a triangular prism with

`Mode`

`.PRIVATE`

and then later use the faces of this object to cut holes in a sphere.width, thickness = 80.0, 10.0 with BuildPart() as ex28: with BuildSketch() as ex28_sk: RegularPolygon(radius=width / 4, side_count=3) ex28_ex = extrude(amount=thickness, mode=Mode.PRIVATE) midfaces = ex28_ex.faces().group_by(Axis.Z)[1] Sphere(radius=width / 2) for face in midfaces: with Locations(face): Hole(thickness / 2)

**Algebra mode**We create a triangular prism and then later use the faces of this object to cut holes in a sphere.

width, thickness = 80.0, 10.0 sk28 = RegularPolygon(radius=width / 4, side_count=3) tmp28 = extrude(sk28, thickness) ex28 = Sphere(radius=width / 2) for p in [Plane(face) for face in tmp28.faces().group_by(Axis.Z)[1]]: ex28 -= p * Hole(thickness / 2, depth=width)

We are able to create multiple workplanes by looping over the list of faces.

## 29. The Classic OCC Bottle

build123d is based on the OpenCascade.org (OCC) modeling Kernel. Those who are familiar with OCC know about the famous ‘bottle’ example. We use a 3D Offset and the openings parameter to create the bottle opening.

**Builder mode**L, w, t, b, h, n = 60.0, 18.0, 9.0, 0.9, 90.0, 6.0 with BuildPart() as ex29: with BuildSketch(Plane.XY.offset(-b)) as ex29_ow_sk: with BuildLine() as ex29_ow_ln: l1 = Line((0, 0), (0, w / 2)) l2 = ThreePointArc(l1 @ 1, (L / 2.0, w / 2.0 + t), (L, w / 2.0)) l3 = Line(l2 @ 1, ((l2 @ 1).X, 0, 0)) mirror(ex29_ow_ln.line) make_face() extrude(amount=h + b) fillet(ex29.edges(), radius=w / 6) with BuildSketch(ex29.faces().sort_by(Axis.Z)[-1]): Circle(t) extrude(amount=n) necktopf = ex29.faces().sort_by(Axis.Z)[-1] offset(ex29.solids()[0], amount=-b, openings=necktopf)

**Algebra mode**L, w, t, b, h, n = 60.0, 18.0, 9.0, 0.9, 90.0, 8.0 l1 = Line((0, 0), (0, w / 2)) l2 = ThreePointArc(l1 @ 1, (L / 2.0, w / 2.0 + t), (L, w / 2.0)) l3 = Line(l2 @ 1, ((l2 @ 1).X, 0, 0)) ln29 = l1 + l2 + l3 ln29 += mirror(ln29) sk29 = make_face(ln29) ex29 = extrude(sk29, -(h + b)) ex29 = fillet(ex29.edges(), radius=w / 6) neck = Plane(ex29.faces().sort_by().last) * Circle(t) ex29 += extrude(neck, n) necktopf = ex29.faces().sort_by().last ex29 = offset(ex29, -b, openings=necktopf)

## 30. Bezier Curve

Here `pts`

is used as an input to both `Polyline`

and
`Bezier`

and `wts`

to Bezier alone. These two together
create a closed line that is made into a face and extruded.

**Builder mode**pts = [ (0, 0), (20, 20), (40, 0), (0, -40), (-60, 0), (0, 100), (100, 0), ] wts = [ 1.0, 1.0, 2.0, 3.0, 4.0, 2.0, 1.0, ] with BuildPart() as ex30: with BuildSketch() as ex30_sk: with BuildLine() as ex30_ln: l0 = Polyline(pts) l1 = Bezier(pts, weights=wts) make_face() extrude(amount=10)

**Algebra mode**pts = [ (0, 0), (20, 20), (40, 0), (0, -40), (-60, 0), (0, 100), (100, 0), ] wts = [ 1.0, 1.0, 2.0, 3.0, 4.0, 2.0, 1.0, ] ex30_ln = Polyline(pts) + Bezier(pts, weights=wts) ex30_sk = make_face(ex30_ln) ex30 = extrude(ex30_sk, -10)

## 31. Nesting Locations

Locations contexts can be nested to create groups of shapes. Here 24 triangles, 6 squares, and
1 hexagon are created and then extruded. Notably `PolarLocations`

rotates any “children” groups by default.

**Builder mode**a, b, c = 80.0, 5.0, 3.0 with BuildPart() as ex31: with BuildSketch() as ex31_sk: with PolarLocations(a / 2, 6): with GridLocations(3 * b, 3 * b, 2, 2): RegularPolygon(b, 3) RegularPolygon(b, 4) RegularPolygon(3 * b, 6, rotation=30) extrude(amount=c)

**Algebra mode**a, b, c = 80.0, 5.0, 3.0 ex31 = Rot(Z=30) * RegularPolygon(3 * b, 6) ex31 += PolarLocations(a / 2, 6) * ( RegularPolygon(b, 4) + GridLocations(3 * b, 3 * b, 2, 2) * RegularPolygon(b, 3) ) ex31 = extrude(ex31, 3)

## 32. Python For-Loop

In this example, a standard python for-loop is used along with a list of faces extracted from a sketch
to progressively modify the extrusion amount. There are 7 faces in the sketch, so this results in 7
separate calls to `extrude()`

.

**Builder mode**`Mode`

`.PRIVATE`

is used in`BuildSketch`

to avoid adding these faces until the for-loop.a, b, c = 80.0, 10.0, 1.0 with BuildPart() as ex32: with BuildSketch(mode=Mode.PRIVATE) as ex32_sk: RegularPolygon(2 * b, 6, rotation=30) with PolarLocations(a / 2, 6): RegularPolygon(b, 4) for idx, obj in enumerate(ex32_sk.sketch.faces()): add(obj) extrude(amount=c + 3 * idx)

**Algebra mode**a, b, c = 80.0, 10.0, 1.0 ex32_sk = RegularPolygon(2 * b, 6, rotation=30) ex32_sk += PolarLocations(a / 2, 6) * RegularPolygon(b, 4) ex32 = Part() + [extrude(obj, c + 3 * idx) for idx, obj in enumerate(ex32_sk.faces())]

## 33. Python Function and For-Loop

Building on the previous example, a standard python function is used to return a sketch as a function of several inputs to progressively modify the size of each square.

**Builder mode**The function returns a

`BuildSketch`

.a, b, c = 80.0, 5.0, 1.0 def square(rad, loc): with BuildSketch() as sk: with Locations(loc): RegularPolygon(rad, 4) return sk.sketch with BuildPart() as ex33: with BuildSketch(mode=Mode.PRIVATE) as ex33_sk: locs = PolarLocations(a / 2, 6) for i, j in enumerate(locs): add(square(b + 2 * i, j)) for idx, obj in enumerate(ex33_sk.sketch.faces()): add(obj) extrude(amount=c + 2 * idx)

**Algebra mode**The function returns a

`Sketch`

object.a, b, c = 80.0, 5.0, 1.0 def square(rad, loc): return loc * RegularPolygon(rad, 4) ex33 = Part() + [ extrude(square(b + 2 * i, loc), c + 2 * i) for i, loc in enumerate(PolarLocations(a / 2, 6)) ]

## 34. Embossed and Debossed Text

**Builder mode**The text “Hello” is placed on top of a rectangle and embossed (raised) by placing a BuildSketch on the top face (

`topf`

). Note that`Align`

is used to control the text placement. We re-use the`topf`

variable to select the same face and deboss (indented) the text “World”. Note that if we simply ran`BuildSketch(ex34.faces().sort_by(Axis.Z)[-1])`

for both`ex34_sk1 & 2`

it would incorrectly locate the 2nd “World” text on the top of the “Hello” text.length, width, thickness, fontsz, fontht = 80.0, 60.0, 10.0, 25.0, 4.0 with BuildPart() as ex34: Box(length, width, thickness) topf = ex34.faces().sort_by(Axis.Z)[-1] with BuildSketch(topf) as ex34_sk: Text("Hello", font_size=fontsz, align=(Align.CENTER, Align.MIN)) extrude(amount=fontht) with BuildSketch(topf) as ex34_sk2: Text("World", font_size=fontsz, align=(Align.CENTER, Align.MAX)) extrude(amount=-fontht, mode=Mode.SUBTRACT)

**Algebra mode**The text “Hello” is placed on top of a rectangle and embossed (raised) by placing a sketch on the top face (

`topf`

). Note that`Align`

is used to control the text placement. We re-use the`topf`

variable to select the same face and deboss (indented) the text “World”.length, width, thickness, fontsz, fontht = 80.0, 60.0, 10.0, 25.0, 4.0 ex34 = Box(length, width, thickness) plane = Plane(ex34.faces().sort_by().last) ex34_sk = plane * Text("Hello", font_size=fontsz, align=(Align.CENTER, Align.MIN)) ex34 += extrude(ex34_sk, amount=fontht) ex34_sk2 = plane * Text("World", font_size=fontsz, align=(Align.CENTER, Align.MAX)) ex34 -= extrude(ex34_sk2, amount=-fontht)

## 35. Slots

**Builder mode**Here we create a

`SlotCenterToCenter`

and then use a`BuildLine`

and`RadiusArc`

to create an arc for two instances of`SlotArc`

.length, width, thickness = 80.0, 60.0, 10.0 with BuildPart() as ex35: Box(length, length, thickness) topf = ex35.faces().sort_by(Axis.Z)[-1] with BuildSketch(topf) as ex35_sk: SlotCenterToCenter(width / 2, 10) with BuildLine(mode=Mode.PRIVATE) as ex35_ln: RadiusArc((-width / 2, 0), (0, width / 2), radius=width / 2) SlotArc(arc=ex35_ln.edges()[0], height=thickness, rotation=0) with BuildLine(mode=Mode.PRIVATE) as ex35_ln2: RadiusArc((0, -width / 2), (width / 2, 0), radius=-width / 2) SlotArc(arc=ex35_ln2.edges()[0], height=thickness, rotation=0) extrude(amount=-thickness, mode=Mode.SUBTRACT)

**Algebra mode**Here we create a

`SlotCenterToCenter`

and then use a`RadiusArc`

to create an arc for two instances of`SlotArc`

.length, width, thickness = 80.0, 60.0, 10.0 ex35 = Box(length, length, thickness) plane = Plane(ex35.faces().sort_by().last) ex35_sk = SlotCenterToCenter(width / 2, 10) ex35_ln = RadiusArc((-width / 2, 0), (0, width / 2), radius=width / 2) ex35_sk += SlotArc(arc=ex35_ln.edges()[0], height=thickness) ex35_ln2 = RadiusArc((0, -width / 2), (width / 2, 0), radius=-width / 2) ex35_sk += SlotArc(arc=ex35_ln2.edges()[0], height=thickness) ex35 -= extrude(plane * ex35_sk, -thickness)

## 36. Extrude Until

Sometimes you will want to extrude until a given face that could be non planar or
where you might not know easily the distance you have to extrude to. In such
cases you can use `extrude()`

`Until`

with `Until.NEXT`

or `Until.LAST`

.

**Builder mode**rad, rev = 6, 50 with BuildPart() as ex36: with BuildSketch() as ex36_sk: with Locations((0, rev)): Circle(rad) revolve(axis=Axis.X, revolution_arc=180) with BuildSketch() as ex36_sk2: Rectangle(rad, rev) extrude(until=Until.NEXT)

**Algebra mode**rad, rev = 6, 50 ex36_sk = Pos(0, rev) * Circle(rad) ex36 = revolve(axis=Axis.X, profiles=ex36_sk, revolution_arc=180) ex36_sk2 = Rectangle(rad, rev) ex36 += extrude(ex36_sk2, until=Until.NEXT, target=ex36)