Skriptgenerierte Objekte

From FreeCAD Documentation
Jump to navigation Jump to search
This page is a translated version of the page Scripted objects and the translation is 40% complete.
Other languages:
Bahasa Indonesia • ‎Deutsch • ‎English • ‎Türkçe • ‎español • ‎français • ‎italiano • ‎polski • ‎português • ‎română • ‎svenska • ‎čeština • ‎русский • ‎中文(中国大陆)‎

Einführung

Neben den Standard Objekttypen wie Anmerkungen, Netze und Teileobjekte bietet FreeCAD auch die erstaunliche Möglichkeit, 100% in python geschriebene parametrische Objekte zu erstellen, die als Python Funktionen bezeichnet werden. Diese Objekte verhalten sich genau wie jedes andere FreeCAD Objekt und werden beim Speichern/Laden von Dateien automatisch gespeichert und wiederhergestellt.

Eine Besonderheit muss beachtet werden: Aus Sicherheitsgründen enthalten FreeCAD Dateien niemals eingebetteten Code. Der Python Code, den du zum Erstellen von parametrischen Objekten schreibst, wird niemals innerhalb einer Datei gespeichert. Das bedeutet, dass, wenn du eine Datei, die ein solches Objekt enthält, auf einem anderen Rechner öffnest, wenn dieser Python Code auf diesem Rechner nicht verfügbar ist, das Objekt nicht vollständig neu erstellt wird. Wenn du solche Objekte an andere weitergibst, musst du auch dein Python Skript weitergeben, z. B. als Makro.

Hinweis: Es ist möglich, Python Code in eine FreeCAD Datei zu packen, indem man json mit einem App::PropertyPythonObject serialisiert, aber dieser Code kann nie direkt ausgeführt werden und hat daher für unseren Zweck hier wenig Nutzen.

Python Funktionen folgen der gleichen Regel wie alle FreeCAD Funktionen: Sie sind in App- und einen GUI Teile getrennt. Der App Teil, das Dokument Objekt, definiert die Geometrie unseres Objekts, während sein GUI Teil, das View Provider Objekt, definiert, wie das Objekt auf dem Bildschirm gezeichnet wird. Das Ansichtsprovider Objekt ist, wie jede andere FreeCAD Funktion, nur verfügbar, wenn Sie FreeCAD in seiner eigenen GUI ausführen. Es stehen mehrere Eigenschaften und Methoden zur Verfügung, um Ihr Objekt zu erstellen. Die Eigenschaften müssen zu einem der vordefinierten Eigenschaftstypen gehören, die FreeCAD anbietet, und werden im Eigenschaften Ansichtsfenster angezeigt, damit sie vom Benutzer bearbeitet werden können. Auf diese Weise sind FeaturePython Objekte wirklich und vollständig parametrisch. Du kannst Eigenschaften für das Objekt und sein Ansichtsobjekt getrennt definieren.

Grundlegendes Beispiel

Das folgende Beispiel ist zusammen mit einigen anderen Beispielen in der src/Mod/TemplatePyMod/FeaturePython.py Datei zu finden:

'''Examples for a feature class and its view provider.'''

import FreeCAD, FreeCADGui
from pivy import coin

class Box:
    def __init__(self, obj):
        '''Add some custom properties to our box feature'''
        obj.addProperty("App::PropertyLength","Length","Box","Length of the box").Length=1.0
        obj.addProperty("App::PropertyLength","Width","Box","Width of the box").Width=1.0
        obj.addProperty("App::PropertyLength","Height","Box", "Height of the box").Height=1.0
        obj.Proxy = self
   
    def onChanged(self, fp, prop):
        '''Do something when a property has changed'''
        FreeCAD.Console.PrintMessage("Change property: " + str(prop) + "\n")
 
    def execute(self, fp):
        '''Do something when doing a recomputation, this method is mandatory'''
        FreeCAD.Console.PrintMessage("Recompute Python Box feature\n")

class ViewProviderBox:
    def __init__(self, obj):
        '''Set this object to the proxy object of the actual view provider'''
        obj.addProperty("App::PropertyColor","Color","Box","Color of the box").Color=(1.0,0.0,0.0)
        obj.Proxy = self
 
    def attach(self, obj):
        '''Setup the scene sub-graph of the view provider, this method is mandatory'''
        self.shaded = coin.SoGroup()
        self.wireframe = coin.SoGroup()
        self.scale = coin.SoScale()
        self.color = coin.SoBaseColor()
       
        data=coin.SoCube()
        self.shaded.addChild(self.scale)
        self.shaded.addChild(self.color)
        self.shaded.addChild(data)
        obj.addDisplayMode(self.shaded,"Shaded");
        style=coin.SoDrawStyle()
        style.style = coin.SoDrawStyle.LINES
        self.wireframe.addChild(style)
        self.wireframe.addChild(self.scale)
        self.wireframe.addChild(self.color)
        self.wireframe.addChild(data)
        obj.addDisplayMode(self.wireframe,"Wireframe");
        self.onChanged(obj,"Color")
 
    def updateData(self, fp, prop):
        '''If a property of the handled feature has changed we have the chance to handle this here'''
        # fp is the handled feature, prop is the name of the property that has changed
        l = fp.getPropertyByName("Length")
        w = fp.getPropertyByName("Width")
        h = fp.getPropertyByName("Height")
        self.scale.scaleFactor.setValue(float(l),float(w),float(h))
        pass
 
    def getDisplayModes(self,obj):
        '''Return a list of display modes.'''
        modes=[]
        modes.append("Shaded")
        modes.append("Wireframe")
        return modes
 
    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):
        '''Here we can do something when a single property got changed'''
        FreeCAD.Console.PrintMessage("Change property: " + str(prop) + "\n")
        if prop == "Color":
            c = vp.getPropertyByName("Color")
            self.color.rgb.setValue(c[0],c[1],c[2])
 
    def getIcon(self):
        '''Return the icon in XPM 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):
        '''When saving the document this object gets stored using Python's json module.\
                Since we have some un-serializable parts here -- the Coin stuff -- we must define this method\
                to return a tuple of all serializable objects or None.'''
        return None
 
    def __setstate__(self,state):
        '''When restoring the serialized object from document we have the chance to set some internals here.\
                Since no data were serialized nothing needs to be done here.'''
        return None


def makeBox():
    FreeCAD.newDocument()
    a=FreeCAD.ActiveDocument.addObject("App::FeaturePython","Box")
    Box(a)
    ViewProviderBox(a.ViewObject)

makeBox()

Things to note

If your object relies on being recomputed as soon as it is created, you must do this manually in the __init__ function as it is not called automatically. This example does not require it because the onChanged method of the Box class has the same effect as the execute function, but the examples below rely on being recomputed before anything is displayed in the 3D view. In the examples, this is done manually with ActiveDocument.recompute() but in more complex scenarios you need to decide where to recompute either the whole document or the FeaturePython object.

This example produces a number of exception stack traces in the report view window. This is because the onChanged method of the Box class is called each time a property is added in __init__. When the first one is added, the Width and Height properties don't exist yet and so the attempt to access them fails.

Eine Erklärung von __getstate__ und __setstate__ findest du im Forumsbeitrag obj.Proxy.Type ist ein Verzeichnis, keine Zeichenfolge.

Verfügbare Methoden

Siehe FunktionPython Methoden für die vollständige Referenz.

Verfügbare Eigenschaften

Eigenschaften sind die wahren Bausteine von FeaturePython-Gegenständen. Durch ist der Benutzer im Stande, mit einem Objekt zu interagieren und es zu ändern. Nach dem Erstellen eines neuen FeaturePython-Objekts in Ihrem Dokument( a=FreeCAD.ActiveDocument.addObject("App::FeaturePython","Box") ), können eine Liste der verfügbaren Eigenschaften bekommen, indem Sie folgendes eingeben:

obj.supportedProperties()

Du erhälst eine Liste der verfügbaren Eigenschaften, die auf der Seite FunktionsPython benutzerdefinierte Eigenschaften näher beschrieben werden:

Beim Hinzufügen von Eigenschaften zu benutzerdefinierten Objekte, achten Sie bitte auf folgendes:

  • Verwenden Sie keine Zeichen "<" oder ">" in den Eigenschaftes-Beschreibungen (das würde den XML-Teil in der .Fcstd-Datei zerbrechen)
  • Eigenschaften werden alphabetisch in einer .fcstd Datei gespeichert. Wenn Sie eine Form("Shape") in Ihren Eigenschaften haben, wird jede Eigenschaft, deren Name in alphabetischen Reihenfolge nach "Shape" kommt, auch nach der Form geladen, was zu seltsamen Verhaltensweisen führen kann.

A complete list of property attributes can be seen in the PropertyStandard C++ header file. For instance, if you want to allow the user to enter only a limited range of values (e.g. using PropertyIntegerConstraint), in Python you will assign a tuple containing not only the property value, but also the lower and upper limit as well as the stepsize, as below:

prop = (value, lower, upper, stepsize)

Eigenschaftstyp

Standardmäßig können die Eigenschaften aktualisiert werden. Es ist möglich, die Eigenschaften schreibgeschützt zu machen, zum Beispiel für den Fall, dass man das Ergebnis einer Methode anzeigen möchte. Es ist auch möglich, die Eigenschaft auszublenden. Der Eigenschaftstyp kann festgelegt werden mit

obj.setEditorMode("MyPropertyName", mode)

wobei mode ein kurzer int ist, der gesetzt werden kann auf:

0 -- Standardmodus, Lesen und Schreiben
1 -- Nur-Lesen
2 -- Versteckt

The EditorModes are not set at FreeCAD file reload. This could to be done by the __setstate__ function. See http://forum.freecadweb.org/viewtopic.php?f=18&t=13460&start=10#p108072. By using the setEditorMode the properties are only read only in PropertyEditor. They could still be changed from python. To really make them read only the setting has to be passed directly inside the addProperty function. See http://forum.freecadweb.org/viewtopic.php?f=18&t=13460&start=20#p109709 for an example.

Using the direct setting in the addProperty function, you also have more possibilities. In particular, an interesting one is mark a property as an output property. This way FreeCAD won't mark the feature as touched when changing it (so no need to recompute).

Example of output property (see also https://forum.freecadweb.org/viewtopic.php?t=24928):

obj.addProperty("App::PropertyString","MyCustomProperty","","",8)

The property types that can be set at last parameter of the addProperty function are:

 0 -- Prop_None, No special property type
 1 -- Prop_ReadOnly, Property is read-only in the editor
 2 -- Prop_Transient, Property won't be saved to file
 4 -- Prop_Hidden, Property won't appear in the editor
 8 -- Prop_Output, Modified property doesn't touch its parent container
 16 -- Prop_NoRecompute, Modified property doesn't touch its container for recompute


You can find these different property types defined in the source code C++ header for PropertyContainer

Andere komplexere Beispiele

Dieses Beispiel macht vom Part Modul Gebrauch, um ein Oktaeder zu schaffen, erstellt dann seine coin Darstellung mit pivy.

Das Erste ist das Documentobjekt selbst:

import FreeCAD, FreeCADGui, Part
import pivy
from pivy import coin

class Octahedron:
  def __init__(self, obj):
     "Add some custom properties to our box feature"
     obj.addProperty("App::PropertyLength","Length","Octahedron","Length of the octahedron").Length=1.0
     obj.addProperty("App::PropertyLength","Width","Octahedron","Width of the octahedron").Width=1.0
     obj.addProperty("App::PropertyLength","Height","Octahedron", "Height of the octahedron").Height=1.0
     obj.addProperty("Part::PropertyPartShape","Shape","Octahedron", "Shape of the octahedron")
     obj.Proxy = self

  def execute(self, fp):
     # Define six vetices for the shape
     v1 = FreeCAD.Vector(0,0,0)
     v2 = FreeCAD.Vector(fp.Length,0,0)
     v3 = FreeCAD.Vector(0,fp.Width,0)
     v4 = FreeCAD.Vector(fp.Length,fp.Width,0)
     v5 = FreeCAD.Vector(fp.Length/2,fp.Width/2,fp.Height/2)
     v6 = FreeCAD.Vector(fp.Length/2,fp.Width/2,-fp.Height/2)
     
     # Make the wires/faces
     f1 = self.make_face(v1,v2,v5)
     f2 = self.make_face(v2,v4,v5)
     f3 = self.make_face(v4,v3,v5)
     f4 = self.make_face(v3,v1,v5)
     f5 = self.make_face(v2,v1,v6)
     f6 = self.make_face(v4,v2,v6)
     f7 = self.make_face(v3,v4,v6)
     f8 = self.make_face(v1,v3,v6)
     shell=Part.makeShell([f1,f2,f3,f4,f5,f6,f7,f8])
     solid=Part.makeSolid(shell)
     fp.Shape = solid

  # helper mehod to create the faces
  def make_face(self,v1,v2,v3):
     wire = Part.makePolygon([v1,v2,v3,v1])
     face = Part.Face(wire)
     return face

Dann haben wir das View Provider Objekt, das für die Darstellung des Objekts in der 3D Szene verantwortlich ist:

class ViewProviderOctahedron:
  def __init__(self, obj):
     "Set this object to the proxy object of the actual view provider"
     obj.addProperty("App::PropertyColor","Color","Octahedron","Color of the octahedron").Color=(1.0,0.0,0.0)
     obj.Proxy = self

  def attach(self, obj):
     "Setup the scene sub-graph of the view provider, this method is mandatory"
     self.shaded = coin.SoGroup()
     self.wireframe = coin.SoGroup()
     self.scale = coin.SoScale()
     self.color = coin.SoBaseColor()

     self.data=coin.SoCoordinate3()
     self.face=coin.SoIndexedLineSet()

     self.shaded.addChild(self.scale)
     self.shaded.addChild(self.color)
     self.shaded.addChild(self.data)
     self.shaded.addChild(self.face)
     obj.addDisplayMode(self.shaded,"Shaded");
     style=coin.SoDrawStyle()
     style.style = coin.SoDrawStyle.LINES
     self.wireframe.addChild(style)
     self.wireframe.addChild(self.scale)
     self.wireframe.addChild(self.color)
     self.wireframe.addChild(self.data)
     self.wireframe.addChild(self.face)
     obj.addDisplayMode(self.wireframe,"Wireframe");
     self.onChanged(obj,"Color")

  def updateData(self, fp, prop):
     "If a property of the handled feature has changed we have the chance to handle this here"
     # fp is the handled feature, prop is the name of the property that has changed
     if prop == "Shape":
        s = fp.getPropertyByName("Shape")
        self.data.point.setNum(6)
        cnt=0
        for i in s.Vertexes:
           self.data.point.set1Value(cnt,i.X,i.Y,i.Z)
           cnt=cnt+1
        
        self.face.coordIndex.set1Value(0,0)
        self.face.coordIndex.set1Value(1,1)
        self.face.coordIndex.set1Value(2,2)
        self.face.coordIndex.set1Value(3,-1)

        self.face.coordIndex.set1Value(4,1)
        self.face.coordIndex.set1Value(5,3)
        self.face.coordIndex.set1Value(6,2)
        self.face.coordIndex.set1Value(7,-1)

        self.face.coordIndex.set1Value(8,3)
        self.face.coordIndex.set1Value(9,4)
        self.face.coordIndex.set1Value(10,2)
        self.face.coordIndex.set1Value(11,-1)

        self.face.coordIndex.set1Value(12,4)
        self.face.coordIndex.set1Value(13,0)
        self.face.coordIndex.set1Value(14,2)
        self.face.coordIndex.set1Value(15,-1)

        self.face.coordIndex.set1Value(16,1)
        self.face.coordIndex.set1Value(17,0)
        self.face.coordIndex.set1Value(18,5)
        self.face.coordIndex.set1Value(19,-1)

        self.face.coordIndex.set1Value(20,3)
        self.face.coordIndex.set1Value(21,1)
        self.face.coordIndex.set1Value(22,5)
        self.face.coordIndex.set1Value(23,-1)

        self.face.coordIndex.set1Value(24,4)
        self.face.coordIndex.set1Value(25,3)
        self.face.coordIndex.set1Value(26,5)
        self.face.coordIndex.set1Value(27,-1)

        self.face.coordIndex.set1Value(28,0)
        self.face.coordIndex.set1Value(29,4)
        self.face.coordIndex.set1Value(30,5)
        self.face.coordIndex.set1Value(31,-1)

  def getDisplayModes(self,obj):
     "Return a list of display modes."
     modes=[]
     modes.append("Shaded")
     modes.append("Wireframe")
     return modes

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

  def setDisplayMode(self,mode):
     return mode

  def onChanged(self, vp, prop):
     "Here we can do something when a single property got changed"
     FreeCAD.Console.PrintMessage("Change property: " + str(prop) + "\n")
     if prop == "Color":
        c = vp.getPropertyByName("Color")
        self.color.rgb.setValue(c[0],c[1],c[2])

  def getIcon(self):
     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):
     return None

  def __setstate__(self,state):
     return None

Schließlich, sobald unser Objekt und sein Viewobjekt definiert sind, müssen wir sie nur noch aufrufen (Der Code der Octahedron Klasse und der Viewprovider Klasse könnte direkt in die FreeCAD Python Konsole kopiert werden):

FreeCAD.newDocument()
a=FreeCAD.ActiveDocument.addObject("App::FeaturePython","Octahedron")
Octahedron(a)
ViewProviderOctahedron(a.ViewObject)

Objekte auswählbar machen

Wenn du dein Objekt oder zumindest einen Teil davon durch Anklicken im Ansichtsfenster auswählbar machen möchtest, musst du seine coin Geometrie in einen SoFCSelection Knoten aufnehmen. Wenn dein Objekt eine komplexe Darstellung hat, mit Widgets, Anmerkungen usw., möchtest du vielleicht nur einen Teil davon in eine SoFCSelection einschließen. Alles, was eine SoFCSelection ist, wird von FreeCAD ständig gescannt, um Auswahl/Vorwahl zu erkennen, daher ist es sinnvoll, es nicht mit unnötigem Scannen zu überlasten.

Once the parts of the scenegraph that are to be selectable are inside SoFCSelection nodes, you then need to provide two methods to handle the selection path. The selection path can take the form of a string giving the names of each element in the path, or of an array of scenegraph objects. The two methods you provide are getDetailPath, which converts from a string path to an array of scenegraph objects, and getElementPicked, which takes an element which has been clicked on in the scenegraph and returns its string name (note, not its string path).

Hier ist das obige Molekülbeispiel, angepasst, um die Elemente des Moleküls auswählbar zu machen:

class Molecule:
    def __init__(self, obj):
        ''' Add two point properties '''
        obj.addProperty("App::PropertyVector","p1","Line","Start point")
        obj.addProperty("App::PropertyVector","p2","Line","End point").p2=FreeCAD.Vector(5,0,0)

        obj.Proxy = self

    def onChanged(self, fp, prop):
        if prop == "p1" or prop == "p2":
            ''' Print the name of the property that has changed '''
            fp.Shape = Part.makeLine(fp.p1,fp.p2)

    def execute(self, fp):
        ''' Print a short message when doing a recomputation, this method is mandatory '''
        fp.Shape = Part.makeLine(fp.p1,fp.p2)

class ViewProviderMolecule:
    def __init__(self, obj):
        ''' Set this object to the proxy object of the actual view provider '''
        obj.Proxy = self
        self.ViewObject = obj
        sep1=coin.SoSeparator()
        sel1 = coin.SoType.fromName('SoFCSelection').createInstance()
        # sel1.policy.setValue(coin.SoSelection.SHIFT)
        sel1.ref()
        sep1.addChild(sel1)
        self.trl1=coin.SoTranslation()
        sel1.addChild(self.trl1)
        sel1.addChild(coin.SoSphere())
        sep2=coin.SoSeparator()
        sel2 = coin.SoType.fromName('SoFCSelection').createInstance()
        sel2.ref()
        sep2.addChild(sel2)
        self.trl2=coin.SoTranslation()
        sel2.addChild(self.trl2)
        sel2.addChild(coin.SoSphere())
        obj.RootNode.addChild(sep1)
        obj.RootNode.addChild(sep2)
        self.updateData(obj.Object, 'p2')
        self.sel1 = sel1
        self.sel2 = sel2

    def getDetailPath(self, subname, path, append):
        vobj = self.ViewObject
        if append:
            path.append(vobj.RootNode)
            path.append(vobj.SwitchNode)

            mode = vobj.SwitchNode.whichChild.getValue()
            if mode >= 0:
                mode = vobj.SwitchNode.getChild(mode)
                path.append(mode)
                sub = Part.splitSubname(subname)[-1]
                if sub == 'Atom1':
                    path.append(self.sel1)
                elif sub == 'Atom2':
                    path.append(self.sel2)
                else:
                    path.append(mode.getChild(0))
        return True

    def getElementPicked(self, pp):
        path = pp.getPath()
        if path.findNode(self.sel1) >= 0:
            return 'Atom1'
        if path.findNode(self.sel2) >= 0:
            return 'Atom2'
        raise NotImplementedError


    def updateData(self, fp, prop):
        "If a property of the handled feature has changed we have the chance to handle this here"
        # fp is the handled feature, prop is the name of the property that has changed
        if prop == "p1":
            p = fp.getPropertyByName("p1")
            self.trl1.translation=(p.x,p.y,p.z)
        elif prop == "p2":
            p = fp.getPropertyByName("p2")
            self.trl2.translation=(p.x,p.y,p.z)

    def __getstate__(self):
        return None

    def __setstate__(self,state):
        return None

def makeMolecule():
    FreeCAD.newDocument()
    a=FreeCAD.ActiveDocument.addObject("Part::FeaturePython","Molecule")
    Molecule(a)
    ViewProviderMolecule(a.ViewObject)
    FreeCAD.ActiveDocument.recompute()

Arbeiten mit einfachen Formen

Erstellen Sie einfach einen SoFCSelection Knoten, dann fügen Sie Ihre Geometrie-Knoten dazu hinzu, dann fügen Sie alles zu Ihrem Hauptknoten hinzu, anstatt Ihre Geometrie-Knoten direkt einzufügen. Die Form wird mittels der FreeCAD Standard-Form-Darstellung angezeigt:

import FreeCAD as App
import FreeCADGui
import FreeCAD
import Part
class Line:
    def __init__(self, obj):
        '''"App two point properties" '''
        obj.addProperty("App::PropertyVector","p1","Line","Start point")
        obj.addProperty("App::PropertyVector","p2","Line","End point").p2=FreeCAD.Vector(1,0,0)
        obj.Proxy = self

    def execute(self, fp):
        '''"Print a short message when doing a recomputation, this method is mandatory" '''
        fp.Shape = Part.makeLine(fp.p1,fp.p2)

a=FreeCAD.ActiveDocument.addObject("Part::FeaturePython","Line")
Line(a)
a.ViewObject.Proxy=0 # just set it to something different from None (this assignment is needed to run an internal notification)
FreeCAD.ActiveDocument.recompute()

Gleicher Code unter Verwendung von ViewProviderLine

import FreeCAD as App
import FreeCADGui
import FreeCAD
import Part

class Line:
    def __init__(self, obj):
         '''"App two point properties" '''
         obj.addProperty("App::PropertyVector","p1","Line","Start point")
         obj.addProperty("App::PropertyVector","p2","Line","End point").p2=FreeCAD.Vector(100,0,0)
         obj.Proxy = self
   
    def execute(self, fp):
        '''"Print a short message when doing a recomputation, this method is mandatory" '''
        fp.Shape = Part.makeLine(fp.p1,fp.p2)

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

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

a=FreeCAD.ActiveDocument.addObject("Part::FeaturePython","Line")
Line(a)
ViewProviderLine(a.ViewObject)
App.ActiveDocument.recompute()

Szenegraph Struktur

Du hast vielleicht bemerkt, dass die obigen Beispiele deine Szenengraphen auf leicht unterschiedliche Weise aufbauen. Einige verwenden obj.addDisplayMode(node, "modename"), während andere obj.SwitchNode.getChild(x).addChild(y) verwenden.

Each feature in a FreeCAD document is based the following scenegraph structure:

RootNode
 \- SwitchNode
     \- Shaded
      - Wireframe
      - etc

The SwitchNode displays only one of its children, depending on which display mode is selection in FreeCAD.

The examples which use addDisplayMode are constructing their scenegraphs solely out of coin3d scenegraph elements. Under the covers, addDisplayMode adds a new child to the SwitchNode; the name of that node will match the display mode it was passed.

The examples which use SwitchNode.getChild(x).addChild also construct part of their geometry using functions from the Part workbench, such as fp.Shape = Part.makeLine(fp.p1,fp.p2). This constructs the different display mode scenegraphs under the SwitchNode; when we later come to add coin3d elements to the scenegraph, we need to add them to the existing display mode scenegraphs using addChild rather than creating a new child of the SwitchNode.

When using addDisplayMode() to add geometry to the scenegraph, each display mode should have its own node which is passed to addDisplayMode(); don't reuse the same node for this. Doing so will confuse the selection mechanism. It's okay if each display mode's node has the same geometry nodes added below it, just the root of each display mode needs to be distinct.

Here is the above molecule example, adapted to be drawn only with Coin3D scenegraph objects instead of using objects from the Part workbench:

import Part
from pivy import coin

class Molecule:
    def __init__(self, obj):
        ''' Add two point properties '''
        obj.addProperty("App::PropertyVector","p1","Line","Start point")
        obj.addProperty("App::PropertyVector","p2","Line","End point").p2=FreeCAD.Vector(5,0,0)

        obj.Proxy = self

    def onChanged(self, fp, prop):
        pass

    def execute(self, fp):
        ''' Print a short message when doing a recomputation, this method is mandatory '''
        pass

class ViewProviderMolecule:
    def __init__(self, obj):
        ''' Set this object to the proxy object of the actual view provider '''
        self.constructed = False
        obj.Proxy = self
        self.ViewObject = obj

    def attach(self, obj):
        material = coin.SoMaterial()
        material.diffuseColor = (1.0, 0.0, 0.0)
        material.emissiveColor = (1.0, 0.0, 0.0)
        drawStyle = coin.SoDrawStyle()
        drawStyle.pointSize.setValue(10)
        drawStyle.style = coin.SoDrawStyle.LINES
        wireframe = coin.SoGroup()
        shaded = coin.SoGroup()
        self.wireframe = wireframe
        self.shaded = shaded

        self.coords = coin.SoCoordinate3()
        self.coords.point.setValues(0, 2, [FreeCAD.Vector(0, 0, 0), FreeCAD.Vector(1, 0, 0)])
        wireframe += self.coords
        wireframe += drawStyle
        wireframe += material
        shaded += self.coords
        shaded += drawStyle
        shaded += material

        g = coin.SoGroup()
        sel1 = coin.SoType.fromName('SoFCSelection').createInstance()
        sel1.style = 'EMISSIVE_DIFFUSE'
        p1 = coin.SoType.fromName('SoIndexedPointSet').createInstance()
        p1.coordIndex.set1Value(0, 0)
        sel1 += p1
        g += sel1
        wireframe += g
        shaded += g

        g = coin.SoGroup()
        sel2 = coin.SoType.fromName('SoFCSelection').createInstance()
        sel2.style = 'EMISSIVE_DIFFUSE'
        p2 = coin.SoType.fromName('SoIndexedPointSet').createInstance()
        p2.coordIndex.set1Value(0, 1)
        sel2 += p2
        g += sel2
        wireframe += g
        shaded += g

        g = coin.SoGroup()
        sel3 = coin.SoType.fromName('SoFCSelection').createInstance()
        sel3.style = 'EMISSIVE_DIFFUSE'
        p3 = coin.SoType.fromName('SoIndexedLineSet').createInstance()
        p3.coordIndex.setValues(0, 2, [0, 1])
        sel3 += p3
        g += sel3
        wireframe += g
        shaded += g

        obj.addDisplayMode(wireframe, 'Wireframe')
        obj.addDisplayMode(shaded, 'Shaded')

        self.sel1 = sel1
        self.sel2 = sel2
        self.sel3 = sel3
        self.constructed = True
        self.updateData(obj.Object, 'p2')

    def getDetailPath(self, subname, path, append):
        vobj = self.ViewObject
        if append:
            path.append(vobj.RootNode)
            path.append(vobj.SwitchNode)

            mode = vobj.SwitchNode.whichChild.getValue()
            FreeCAD.Console.PrintWarning("getDetailPath: mode {} is active\n".format(mode))
            if mode >= 0:
                mode = vobj.SwitchNode.getChild(mode)
                path.append(mode)
                sub = Part.splitSubname(subname)[-1]
                print(sub)
                if sub == 'Atom1':
                    path.append(self.sel1)
                elif sub == 'Atom2':
                    path.append(self.sel2)
                elif sub == 'Line':
                    path.append(self.sel3)
                else:
                    path.append(mode.getChild(0))
        return True

    def getElementPicked(self, pp):
        path = pp.getPath()
        if path.findNode(self.sel1) >= 0:
            return 'Atom1'
        if path.findNode(self.sel2) >= 0:
            return 'Atom2'
        if path.findNode(self.sel3) >= 0:
            return 'Line'
        raise NotImplementedError


    def updateData(self, fp, prop):
        "If a property of the handled feature has changed we have the chance to handle this here"
        # fp is the handled feature, prop is the name of the property that has changed
        if not self.constructed:
            return
        if prop == "p1":
            p = fp.getPropertyByName("p1")
            self.coords.point.set1Value(0, p)
        elif prop == "p2":
            p = fp.getPropertyByName("p2")
            self.coords.point.set1Value(1, p)

    def getDisplayModes(self, obj):
        return ['Wireframe', 'Shaded']

    def getDefaultDisplayMode(self):
        return 'Shaded'

    def setDisplayMode(self, mode):
        return mode

    def __getstate__(self):
        return None

    def __setstate__(self,state):
        return None

def makeMolecule():
    FreeCAD.newDocument()
    a=FreeCAD.ActiveDocument.addObject("App::FeaturePython","Molecule")
    Molecule(a)
    b=ViewProviderMolecule(a.ViewObject)
    a.touch()
    FreeCAD.ActiveDocument.recompute()
    return a,b

a,b = makeMolecule()

Weitere Informationen

Weitere Seiten:

Interessante Forenbeiträge über geskriptete Objekte:

Zusätzlich zu den hier vorgestellten Beispielen solltedz du einen Blick in den FreeCAD Quellcode src/Mod/TemplatePyMod/FeaturePython.py für weitere Beispiele werfen.