Scripted objects with attachment

Introduction

The purpose of this page is to show a minimal example of Part EditAttachment feature using Scripted objects in Python.

See full and complete minimal example below.

The following GIF demonstrates attaching our custom box to a cylinder, and automatically updating it's position when the cylinder's position changes.

NOTE: The box is our custom scripted object, and the cylinder is a regular FreeCAD object generated from the Part workbench.

Making Scripted Objects Attachable

Add Attach Extension

First, we need to add the Part::AttachExtensionPython extension to our Part::FeaturePython oject in the constructor, or __init__ method, of our custom scripted object.

class Box():
    """Custom Scripted Box Object"""

    def __init__(self, obj):
        self.Type = 'Box'

        obj.Proxy = self
        
        ... custom properties

        # Needed to make this object "attachable"
        obj.addExtension('Part::AttachExtensionPython')

Without adding this code, we'll see the following warning dialog when attaching our custom scripted object to another object.

Update Position Based on Attached Object

Then, in the `execute` method of our custom scripted object, we need to call the `positionBySupport` on our `Part::FeaturePython` object.

class Box:
    
    ...

    def execute(self, obj):
        obj.positionBySupport()
        
        # Assign a Shape to obj
        obj.Shape = Part.makeBox(...)

Without calling positionBySupport, our custom scripted object won't update it's position when the position of the attached-to object changes.

Full and Complete Minimal Example

import FreeCAD as App
import Part


class Box():
    """
    Simple Custom Box Object
    See Also:
        https://wiki.freecadweb.org/FeaturePython_Objects
    """

    def __init__(self, obj):
        """
        Constructor
        Arguments
        ---------
        - obj: an existing document object or an object created with FreeCAD.Document.addObject('Part::FeaturePython', '{name}').
        """

        self.Type = 'Box'

        obj.Proxy = self
        obj.addProperty('App::PropertyLength', 'Length',
                        'Dimensions', 'Box length').Length = 10.0
        obj.addProperty('App::PropertyLength', 'Width',
                        'Dimensions', 'Box width').Width = 10.0
        obj.addProperty('App::PropertyLength', 'Height',
                        'Dimensions', 'Box height').Height = 10.0

        # Needed to make this object "attachable",
        # or able to attach parameterically to other objects
        obj.addExtension('Part::AttachExtensionPython')

    def execute(self, obj):
        """
        Called on document recompute
        """
        # Needed to update position when attached-to object changes position.
        # Reposition object based on Support, MapMode and MapPathParameter properties.
        # Returns True if attachment calculation was successful, False if object is not attached and Placement wasn't updated,
        obj.positionBySupport()

        obj.Shape = Part.makeBox(obj.Length, obj.Width, obj.Height)


def create_box(obj_name, document):
    """
    Create a Box.
    """
    obj = document.addObject('Part::FeaturePython', obj_name)
    Box(obj)
    obj.ViewObject.Proxy = 0  # Mandatory unless ViewProvider is coded
    return obj


document = App.ActiveDocument
if document is None:
    document = App.newDocument('Part Attachment Example')

box = create_box('CustomBox', document)
document.recompute()

References

• Part EditAttachment
• FreeCAD Forum - Parametric attachment of scripted object
• FreeCAD Forum - Port attachment to be an extension
• GitHub - freecad-part-attachment-python-example

Tested With the Following FreeCAD Version

Tested with the following FreeCAD version information:

OS: Ubuntu 18.04.3 LTS
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.18.16146 (Git) AppImage
Build type: Release
Branch: (HEAD detached at 0.18.4)
Hash: 980bf9060e28555fecd9e3462f68ca74007b70f8
Python version: 3.6.7
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/UnitedStates (en_US)

Note: For FreeCAD 0.19 this tutorial needs a minor update:

• The second argument of the`addExtension` method got deprecated.
• For details see https://forum.freecadweb.org/viewtopic.php?f=10&t=54370

Power user documentation

• FreeCAD scripting: Python, Introduction to Python, Python scripting tutorial, FreeCAD Scripting Basics

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• Modules: Builtin modules, Units, Quantity
• Workbenches: Workbench creation, Gui Commands, Commands, Installing more workbenches
• Meshes and Parts: Mesh Scripting, Topological data scripting, Mesh to Part, PythonOCC

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• Parametric objects: Scripted objects, Viewproviders (Custom icon in tree view)
• Scenegraph: Coin (Inventor) scenegraph, Pivy
• Graphical interface: Interface creation, Interface creation completely in Python (1, 2, 3, 4, 5), PySide, PySide examples beginner, intermediate, advanced
• Macros: Macros, How to install macros
• Embedding: Embedding FreeCAD, Embedding FreeCADGui

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• Other: Expressions, Code snippets, Line drawing function, FreeCAD vector math library (deprecated)

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