Creating a FeaturePython Box, Part II

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App::FeaturePython vs. Part::FeaturePython

Up to this pint we've focused on the internal aspects of a Python class built around a FeaturePython object - specifically, an App::FeaturePython object. We've created the object, defined some properties, and added some document-level event callbacks that allow our object to respond to a document recompute with the execute() method.

But we still don't have a box.

We can create one easily just by adding two lines. First, add a new import to the top of the file:

import Part

Then, in execute(), add the following line (you can delete the print() statement):

def execute():
    """
    Called on document recompute
    """

    Part.show(Part.makeBox(obj.Length, obj.Width, obj.Height)


These commands execute python scripts that come with FreeCAD as a default. The makeBox() method generates a new box Shape. The enclosing call to Part.show() adds the Shape to the document tree and makes it visible.

If you have FreeCAD open, reload the box module and create a new box object using box.create() (delete any existing box objects, just to keep things clean).

Notice how a box immediately appears on the screen.

That's because the execute method is called immediately after the box is created, because we force the document to recompute at the end of box.create()

But there's a problem.

It should be pretty obvious. The box itself is represented by an entirely different object than our FeaturePython object. The reason is because Part.show() creates a separate Part::Feature object (dumb shape, same as one created by Part Simple Copy) for the document and assigns the shape created by makeBox() to it.

In fact, if you go to your FeaturePython object and change the dimensions, you'll see another box shape gets created and the old one is left in place. That's not good!

What we want, of course, is a single object that represents a box and resizes the existing box as we change it's properties. We could delete the previous Shape every time we change a property, but we still have two objects - our FeaturePython object and the Shape it generates.

So how do we solve this problem?

First, we need to use the right type of object. To this pint we've been using App::FeaturePython objects. They're great, but they're not intended for use as geometry objects. They're document objects which are meant to do things that don't require a visual in the 3D view. We'll talk more about that later.

For now, we just need to make the following change in create().

Change:

obj = App.ActiveDocument.addObject('App::FeaturePython', obj_name)

to:

obj = App.ActiveDocument.addObject('Part::FeaturePython', obj_name)

Then, in the execute method, change the line:

Part.show(Part.makeBox(obj.Length, obj.Width, obj.Height))

to:

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

Your code should look like this:

import FreeCAD as App
import Part

def create(obj_name):
  """
  Object creation method
  """

  obj = App.ActiveDocument.addObject('Part::FeaturePython', obj_name)

  fpo = box(obj)

  App.ActiveDocument.recompute()

  return fpo

class box():

  def __init__(self, obj):
      """
      Default Constructor
      """

      self.Type = 'box'

      obj.addProperty('App::PropertyString', 'Description', 'Base', 'Box description').Description = ""
      obj.addProperty('App::PropertyLength', 'Length', 'Dimensions', 'Box length').Length = 10.0
      obj.addProperty('App::PropertyLength', 'Width', 'Dimensions', 'Box width').Width = '10 mm'
      obj.addProperty('App::PropertyLength', 'Height', 'Dimensions', 'Box height').Height = '1 cm'

      obj.Proxy = self
      self.Object = obj

  def execute(self, obj):
      """
      Called on document recompute
      """

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

Now, save your changes and switch back to FreeCAD. Delete any existing objects, reload the box module, and create a new box object.

Now take a look at the object in the document tree. See any differences?

The first thing you should see is that the icon changed. It's a cube now.

The second thing you should see (or rather, not see) is the cube. It's not there. And the icon is still gray.

What happened?

The answer is, while we've properly created our box shape and assigned it to a Part::FeaturePython object, before we can make it show up in our 3D view, we need to assign a ViewProvider.

Writing a ViewProvider

A View Provider is the component of an object which allows it to have visual representation in the GUI - specifically in the 3D view. FreeCAD uses an application structure known as 'model-view', which is designed to separate the data (the 'model') from it's visual representation (the 'view'). If you've spent any time working with FreeCAD in Python, you'll likely already be aware of this through the use of two core Python modules: FreeCAD and FreeCADGui (often aliased as 'App' and 'Gui' repectively).

Thus, our FeaturePython Box implementation also requires these elements. Thus far, we've focused purely on the 'model' portion, so now it's time to write the 'view'. Fortunately, most view implementations are simple and require little effort to write, at least to get started. Here's an example ViewProvider, borrowed and slightly modified from [1]


class ViewProviderBox:
   def __init__(self, obj):
       """
       Set this object to the proxy object of the actual view provider
       """
       obj.Proxy = self

   def attach(self, obj):
       """
       Setup the scene sub-graph of the view provider, this method is mandatory
       """
       return

   def updateData(self, fp, prop):
       """
       If a property of the handled feature has changed we have the chance to handle this here
       """
       return

   def getDisplayModes(self,obj):
       """
       Return a list of display modes.
       """
       return None

   def getDefaultDisplayMode(self):
       """
       Return the name of the default display mode. It must be defined in getDisplayModes.
       """
       return "Shaded"

   def setDisplayMode(self,mode):
       """
       Map the display mode defined in attach with those defined in getDisplayModes.
       Since they have the same names nothing needs to be done.
       This method is optional.
       """
       return mode

   def onChanged(self, vp, prop):
       """
       Print the name of the property that has changed
       """

       App.Console.PrintMessage("Change property: " + str(prop) + "\n")

   def getIcon(self):
       """
       Return the icon in XMP format which will appear in the tree view. This method is optional and if not defined a default icon is shown.
       """

       return """
           /* XPM */
           static const char * ViewProviderBox_xpm[] = {
           "16 16 6 1",
           " 	c None",
           ".	c #141010",
           "+	c #615BD2",
           "@	c #C39D55",
           "#	c #000000",
           "$	c #57C355",
           "        ........",
           "   ......++..+..",
           "   .@@@@.++..++.",
           "   .@@@@.++..++.",
           "   .@@  .++++++.",
           "  ..@@  .++..++.",
           "###@@@@ .++..++.",
           "##$.@@$#.++++++.",
           "#$#$.$$$........",
           "#$$#######      ",
           "#$$#$$$$$#      ",
           "#$$#$$$$$#      ",
           "#$$#$$$$$#      ",
           " #$#$$$$$#      ",
           "  ##$$$$$#      ",
           "   #######      "};
           """

   def __getstate__(self):
       """
       Called during document saving.
       """
       return None

   def __setstate__(self,state):
       """"
       Called during document restore.
       """"
       return None


Note in the above code, we also define an XMP icon for this object. Icon design is beyond the scope of this tutorial, but basic icon designs can be managed using open source tools like GIMP, Krita, and Inkscape. The getIcon method is optional, as well. If it is not provided, FreeCAD will provide a default icon.


With out ViewProvider defined, we now need to put it to use to give our object the gift of visualization.

Return to the create() method in your code and add the following near the end:

ViewProviderBox(obj.ViewObject)

This instances the custom ViewProvider class and passes the FeaturePython's built-in ViewObject to it. The ViewObject won't do anything without our custom class implementation, so when the ViewProvider class initializes, it saves a reference to itself in the FeaturePython's ViewObject.Proxy attribute. This way, when FreeCAD needs to render our Box visually, it can find the ViewProvider class to do that.

Now, save the changes and return to FreeCAD. Import or reload the Box module and call box.create().

We still don't see anything, but notice what happened to the icon next to the box object. It's in color! And it has a shape! That's a clue that our ViewProvider is working as expected.

So now, it's time to actually *add* a box.

Return to the code and add the following line to the execute() method:

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

Now save, reload the box module in FreeCAD and create a new box.

You should see a box appear on screen! If it's too big (or maybe doesn't show up at all), click one of the 'ViewFit' buttons to fit it to the 3D view.

Note what we did here that differs from the way it was implemented for App::FeaturePython above. In the execute() method, we called the Part.makeBox() macro and passed it the box properties as before. But rather than call Part.show() on the resulting object (which created a new, separate box object), we simply assigned it to the Shape property of our Part::FeaturePython object instead.

You can even alter the box dimensions by changing the values in the FreeCAD property panel. Give it a try!

Trapping Events

To this point, we haven't explicitly addressed event trapping. Nearly every method of a FeaturePython class serves as a callback accessible to the FeaturePython object (which gets access to our class instance through the Proxy attribute, if you recall).

Below is a list of the callbacks that may be implemented in the basic FeaturePython object:

FeaturePython basic callbacks
execute(self, obj) Called during document recomputes Do not call recompute() from this method (or any method called from execute()) as this causes a nested recompute.
onBeforeChanged(self, obj, prop) Called before a property value is changed prop is the name of the property to be changed, not the property object itself. Property changes cannot be cancelled. Previous / next property values are not simultaneously available for comparison.
onChanged(self, obj, prop) Called after a property is changed prop is the name of the property to be changed, not the property object itself.
onDocumentRestored(self, obj) Called after a document is restored or aFeaturePython object is copied / duplicated. Occasionally, references to the FeaturePython object from the class, or the class from the FeaturePython object may be broken, as the class __init__() method is not called when the object is reconstructed. Adding self.Object = obj or obj.Proxy = self often solves these issues.

In addition, there are two callbacks in the ViewProvider class that may occasionally prove useful:

ViewProvider basic callbacks
udateData(self, obj, prop) Called after a data (model) property is changed obj is a reference to the FeaturePython class instance, not the ViewProvider instance. prop is the name of the property to be changed, not the property object itself.
onChanged(self, vobj, prop) Called after a view property is changed vobj is a reference to the ViewProvider instance. prop is the name of the view property which was changed.


Tip
It is not uncommon to encounter a situation where the Python callbacks are not being triggered as they should. Beginners in this area need to rest assured that the FeaturePython callback system is not fragile or broken. Invariably, when callbacks fail to run, it is because a reference is lost or undefined in the underlying code. If, however, callbacks appear to be breaking with no explanation, providing object / proxy references in the onDocumentRestored() callback (as noted in the first table above) may alleviate these problems. Until you are comfortable with the callback system, it may be useful to add print statements in each callback to print messages to the console as a diagnostic during development.

Adding Complexity