Create a FeaturePython object part II

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  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:

Then, in, add the following line (you can delete the   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  method generates a new box Shape. The enclosing call to  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  (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

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  creates a separate Part::Shape object for the document and assigns the shape created by   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  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.

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

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  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.

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  method, we called the   macro and passed it the box properties as before. But rather than call  on the resulting object (which created a new, separate box object), we simply assigned it to the   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!