###########################
Key Concepts (builder mode)
###########################

There are two primary APIs provided by build123d: builder and algebra. The builder
API may be easier for new users as it provides some assistance and shortcuts; however,
if you know what a Quaternion is you might prefer the algebra API which allows
CAD objects to be created in the style of mathematical equations. Both API can
be mixed in the same model with the exception that the algebra API can't be used
from within a builder context. As with music, there is no "best" genre or API,
use the one you prefer or both if you like.

The following key concepts will help new users understand build123d quickly.

Understanding the Builder Paradigm
==================================

The **Builder** paradigm in build123d provides a powerful and intuitive way to construct 
complex geometric models. At its core, the Builder works like adding a column of numbers 
on a piece of paper: a running "total" is maintained internally as each new object is 
added or modified. This approach simplifies the process of constructing models by breaking 
it into smaller, incremental steps.

How the Builder Works
----------------------

When using a Builder (such as **BuildLine**, **BuildSketch**, or **BuildPart**), the 
following principles apply:

1. **Running Total**:
   - The Builder maintains an internal "total," which represents the current state of 
   the object being built. 
   - Each operation updates this total by combining the new object with the existing one.

2. **Combination Modes**:
   - Just as numbers in a column may have a `+` or `-` sign to indicate addition or 
   subtraction, Builders use **modes** to control how each object is combined with 
   the current total.
   - Common modes include:

     - **ADD**: Adds the new object to the current total.
     - **SUBTRACT**: Removes the new object from the current total.
     - **INTERSECT**: Keeps only the overlapping regions of the new object and the current total.
     - **REPLACE**: Entirely replace the running total.
     - **PRIVATE**: Don't change the running total at all. 

   - The mode can be set dynamically for each operation, allowing for flexible and precise modeling.

3. **Extracting the Result**:
   - At the end of the building process, the final object is accessed through the 
   Builder's attributes, such as ``.line``, ``.sketch``, or ``.part``, depending on 
   the Builder type.
   - For example:
   
     - **BuildLine**: Use ``.line`` to retrieve the final wireframe geometry.
     - **BuildSketch**: Use ``.sketch`` to extract the completed 2D profile.
     - **BuildPart**: Use ``.part`` to obtain the 3D solid.

Example Workflow
-----------------

Here is an example of using a Builder to create a simple part:

.. code-block:: python

    from build123d import *

    # Using BuildPart to create a 3D model
    with BuildPart() as example_part:
        with BuildSketch() as base_sketch:
            Rectangle(20, 20)
        extrude(amount=10)  # Create a base block
        with BuildSketch(Plane(example_part.faces().sort_by(Axis.Z).last)) as cut_sketch:
            Circle(5)
        extrude(amount=-5, mode=Mode.SUBTRACT)  # Subtract a cylinder

    # Access the final part
    result_part = example_part.part

Key Concepts
------------

- **Incremental Construction**:
  Builders allow you to build objects step-by-step, maintaining clarity and modularity.
  
- **Dynamic Mode Switching**:
  The **mode** parameter gives you precise control over how each operation modifies 
  the current total.

- **Seamless Extraction**:
  The Builder paradigm simplifies the retrieval of the final object, ensuring that you 
  always have access to the most up-to-date result.

Analogy: Adding Numbers on Paper
--------------------------------

Think of the Builder as a running tally when adding numbers on a piece of paper:

- Each number represents an operation or object.
- The ``+`` or ``-`` sign corresponds to the **ADD** or **SUBTRACT** mode.
- At the end, the total is the sum of all operations, which you can retrieve by referencing 
  the Builder’s output.

By adopting this approach, build123d ensures a natural, intuitive workflow for constructing 
2D and 3D models.

Builders
========

The three builders, ``BuildLine``, ``BuildSketch``, and ``BuildPart`` are tools to create
new objects - not the objects themselves. Each of the objects and operations applicable
to these builders create objects of the standard CadQuery Direct API, most commonly
``Compound`` objects.  This is opposed to CadQuery's Fluent API which creates objects
of the ``Workplane`` class which frequently needed to be converted back to base
class for further processing.

One can access the objects created by these builders by referencing the appropriate
instance variable. For example:

.. code-block:: python

    with BuildPart() as my_part:
        ...

    show_object(my_part.part)

.. code-block:: python

    with BuildSketch() as my_sketch:
        ...

    show_object(my_sketch.sketch)

.. code-block:: python

    with BuildLine() as my_line:
        ...

    show_object(my_line.line)

Implicit Builder Instance Variables
===================================

One might expect to have to reference a builder's instance variable when using
objects or operations that impact that builder like this:

.. code-block:: python

    with BuildPart() as part_builder:
        Box(part_builder, 10,10,10)

Instead, build123d determines from the scope of the object or operation which
builder it applies to thus eliminating the need for the user to provide this
information - as follows:

.. code-block:: python

    with BuildPart() as part_builder:
        Box(10,10,10)
        with BuildSketch() as sketch_builder:
            Circle(2)

In this example, ``Box`` is in the scope of ``part_builder`` while ``Circle``
is in the scope of ``sketch_builder``.

Workplanes
==========

As build123d is a 3D CAD package one must be able to position objects anywhere. As one
frequently will work in the same plane for a sequence of operations, the first parameter(s)
of the builders is a (sequence of) workplane(s) which is (are) used
to aid in the location of features. The default workplane in most cases is the ``Plane.XY``
where a tuple of numbers represent positions on the x and y axes. However workplanes can
be generated on any plane which allows users to put a workplane where they are working
and then work in local 2D coordinate space.


.. code-block:: python

    with BuildPart(Plane.XY) as example:
        ... # a 3D-part
        with BuildSketch(example.faces().sort_by(sort_by=Axis.Z)[0]) as bottom:
            ...
        with BuildSketch(Plane.XZ) as vertical:
            ...
        with BuildSketch(example.faces().sort_by(sort_by=Axis.Z)[-1]) as top:
            ...

When ``BuildPart`` is invoked it creates the workplane provided as a parameter (which has a
default of the ``Plane.XY``). The ``bottom`` sketch is therefore created on the ``Plane.XY`` but with the
normal reversed to point down. Subsequently the user has created the ``vertical`` (``Plane.XZ``) sketch.
All objects or operations within the scope of a workplane will automatically be orientated with
respect to this plane so the user only has to work with local coordinates.

As shown above, workplanes can be created from faces as well. The ``top`` sketch is
positioned on top of ``example`` by selecting its faces and finding the one with the greatest z value.

One is not limited to a single workplane at a time. In the following example all six
faces of the first box are used to define workplanes which are then used to position
rotated boxes.

.. code-block:: python

    import build123d as bd

    with bd.BuildPart() as bp:
        bd.Box(3, 3, 3)
        with bd.BuildSketch(*bp.faces()):
            bd.Rectangle(1, 2, rotation=45)
        bd.extrude(amount=0.1)

This is the result:

.. image:: boxes_on_faces.svg
  :align: center

.. _location_context_link:

Locations Context
=================

When positioning objects or operations within a builder Location Contexts are used.  These
function in a very similar was to the builders in that they create a context where one or
more locations are active within a scope.  For example:

.. code-block:: python

    with BuildPart():
        with Locations((0,10),(0,-10)):
            Box(1,1,1)
            with GridLocations(x_spacing=5, y_spacing=5, x_count=2, y_count=2):
                Sphere(1)
            Cylinder(1,1)

In this example ``Locations`` creates two positions on the current workplane at (0,10) and (0,-10).
Since ``Box`` is within the scope of ``Locations``, two boxes are created at these locations. The
``GridLocations`` context creates four positions which apply to the ``Sphere``. The ``Cylinder`` is
out of the scope of ``GridLocations`` but in the scope of ``Locations`` so two cylinders are created.

Note that these contexts are creating Location objects not just simple points. The difference
isn't obvious until the ``PolarLocations`` context is used which can also rotate objects within
its scope - much as the hour and minute indicator on an analogue clock.

Also note that the locations are local to the current location(s) - i.e. ``Locations`` can be
nested. It's easy for a user to retrieve the global locations:

.. code-block:: python

    with Locations(Plane.XY, Plane.XZ):
        locs = GridLocations(1, 1, 2, 2)
        for l in locs:
            print(l)

.. code-block::

    Location(p=(-0.50,-0.50,0.00), o=(0.00,-0.00,0.00))
    Location(p=(-0.50,0.50,0.00), o=(0.00,-0.00,0.00))
    Location(p=(0.50,-0.50,0.00), o=(0.00,-0.00,0.00))
    Location(p=(0.50,0.50,0.00), o=(0.00,-0.00,0.00))
    Location(p=(-0.50,-0.00,-0.50), o=(90.00,-0.00,0.00))
    Location(p=(-0.50,0.00,0.50), o=(90.00,-0.00,0.00))
    Location(p=(0.50,0.00,-0.50), o=(90.00,-0.00,0.00))
    Location(p=(0.50,0.00,0.50), o=(90.00,-0.00,0.00))


Operation Inputs
================

When one is operating on an existing object, e.g. adding a fillet to a part,
an iterable of objects is often required (often a ShapeList).

Here is the definition of :meth:`~operations_generic.fillet` to help illustrate:

.. code-block:: python

    def fillet(
        objects: Union[Union[Edge, Vertex], Iterable[Union[Edge, Vertex]]],
        radius: float,
    ):

To use this fillet operation, an edge or vertex or iterable of edges or 
vertices must be provided followed by a fillet radius with or without the keyword as follows:

.. code-block:: python

    with BuildPart() as pipes:
        Box(10, 10, 10, rotation=(10, 20, 30))
        ...
        fillet(pipes.edges(Select.LAST), radius=0.2)

Here the fillet accepts the iterable ShapeList of edges from the last operation of
the ``pipes`` builder and a radius is provided as a keyword argument.

Combination Modes
=================

Almost all objects or operations have a ``mode`` parameter which is defined by the
``Mode`` Enum class as follows:

.. code-block:: python

    class Mode(Enum):
        ADD = auto()
        SUBTRACT = auto()
        INTERSECT = auto()
        REPLACE = auto()
        PRIVATE = auto()

The ``mode`` parameter describes how the user would like the object or operation to
interact with the object within the builder. For example, ``Mode.ADD`` will
integrate a new object(s) in with an existing ``part``.  Note that a part doesn't
necessarily have to be a single object so multiple distinct objects could be added
resulting is multiple objects stored as a ``Compound`` object. As one might expect
``Mode.SUBTRACT``, ``Mode.INTERSECT``, and ``Mode.REPLACE`` subtract, intersect, or replace
(from) the builder's object. ``Mode.PRIVATE`` instructs the builder that this object
should not be combined with the builder's object in any way.

Most commonly, the default ``mode`` is ``Mode.ADD`` but this isn't always true.
For example, the ``Hole`` classes use a default ``Mode.SUBTRACT`` as they remove
a volume from the part under normal circumstances. However, the ``mode`` used in
the ``Hole`` classes can be specified as ``Mode.ADD`` or ``Mode.INTERSECT`` to
help in inspection or debugging.


Using Locations & Rotating Objects
==================================

build123d stores points (to be specific ``Location`` (s)) internally to be used as
positions for the placement of new objects.  By default, a single location
will be created at the origin of the given workplane such that:

.. code-block:: python

    with BuildPart() as pipes:
        Box(10, 10, 10, rotation=(10, 20, 30))

will create a single 10x10x10 box centered at (0,0,0) - by default objects are
centered. One can create multiple objects by pushing points prior to creating
objects as follows:

.. code-block:: python

    with BuildPart() as pipes:
        with Locations((-10, -10, -10), (10, 10, 10)):
            Box(10, 10, 10, rotation=(10, 20, 30))

which will create two boxes.

To orient a part, a ``rotation`` parameter is available on ``BuildSketch``` and
``BuildPart`` APIs. When working in a sketch, the rotation is a single angle in
degrees so the parameter is a float. When working on a part, the rotation is
a three dimensional ``Rotation`` object of the form
``Rotation(<about x>, <about y>, <about z>)`` although a simple three tuple of
floats can be used as input.  As 3D rotations are not cumulative, one can
combine rotations with the `*` operator like this:
``Rotation(10, 20, 30) * Rotation(0, 90, 0)`` to generate any desired rotation.

.. hint::
    Experts Only

    ``Locations`` will accept ``Location`` objects for input which allows one
    to specify both the position and orientation.  However, the orientation
    is often determined by the ``Plane`` that an object was created on.
    ``Rotation`` is a subclass of ``Location`` and therefore will also accept
    a position component.

Builder's Pending Objects
=========================

When a builder exits, it will push the object created back to its parent if
there was one.  Here is an example:

.. code-block:: python

    height, width, thickness, f_rad = 60, 80, 20, 10

    with BuildPart() as pillow_block:
        with BuildSketch() as plan:
            Rectangle(width, height)
            fillet(plan.vertices(), radius=f_rad)
        extrude(amount=thickness)

``BuildSketch`` exits after the ``fillet`` operation and when doing so it transfers
the sketch to the ``pillow_block`` instance of ``BuildPart`` as the internal instance variable
``pending_faces``. This allows the ``extrude`` operation to be immediately invoked as it
extrudes these pending faces into ``Solid`` objects. Likewise, ``loft`` would take all of the
``pending_faces`` and attempt to create a single ``Solid`` object from them.

Normally the user will not need to interact directly with pending objects; however,
one can see pending Edges and Faces with ``<builder_instance>.pending_edges`` and 
``<builder_instance>.pending_faces`` attributes.  In the above example, by adding a 
``print(pillow_block.pending_faces)`` prior to the ``extrude(amount=thickness)`` the
pending ``Face`` from the ``BuildSketch`` will be displayed.