PartDesign Forme legate secondarie

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Lega forme secondarie

Posizione nel menu
Part Design → Crea un riferimento per i(l) sotto oggetti(o)
Avvio veloce
Introdotto nella versione
Vedere anche
Forma legata, Clona


Lo strumento PartDesign SubShapeBinder crea una forma legata che fa riferimento alla geometria da uno o più oggetti principali. Un SubShapeBinder viene in genere utilizzato all'interno di un Corpo per fare riferimento alla geometria esterna al corpo. L'utilizzo della geometria esterna direttamente in un corpo non è consentito e porterà a errori fuori ambito. Ma un SubShapeBinder può essere utilizzato anche senza essere annidato in un Body.

Una Forma Legata Secondaria traccerà il posizionamento relativo della geometria di riferimento, che è utile nel contesto della creazione di assiemi, ma oltre a ciò ha anche un proprio posizionamento.

The referenced geometry can consist of one or multiple elements. Each element can be an individual object (for example a PartDesign Body), a subobject (for example a Part Box inside a Std Part, or a sketch or Feature inside a Body), or a subelement (a face, edge or vertex). Which geometry should be selected depends on the intended purpose of the SubShapeBinder. For a Boolean operation you would need to select a solid. For a Pad operation a face, a sketch or a planar wire can be used. And for the external geometry in a sketch, or to attach a sketch, any combination of subelements may be appropriate. Elements can belong to different parent objects, and can even belong to the Body the SubShapeBinder is nested in. Because a SubShapeBinder is Link-based the referenced geometry can also belong to an external document.

A sinistra: due solidi creati in due corpi separati. A destra: due SubShapeBinders estratti dal primo corpo, importati nel secondo corpo e spostati in una posizione diversa.

I due SubShapeBinders vengono utilizzati per creare un taglio booleano e un pad, con il secondo corpo.


Stesso documento

  1. If there are multiple Bodies in the document: optionally activate the Body the SubShapeBinder should be nested in.
  2. Select the required geometry. Subelements can only be selected in the 3D view.
  3. There are several ways to invoke the tool:
    • Press the PartDesign SubShapeBinder button.
    • Select the Part Design → Create a sub-object(s) shape binder option from the menu.
  4. The SubShapeBinder is created.
  5. If there is only one Body in the document the SubShapeBinder is automatically added to it and the Body is activated. If this is the case and the SubShapeBinder should not be nested, it can be dragged out of the Body and dropped onto the document node in the Tree view.

Documento esterno

  1. If required open the source document (the external document) and the target document. Both documents must have been saved at least once.
  2. If there are multiple Bodies in the target document: optionally activate the Body the SubShapeBinder should be nested in.
  3. Select the required geometry in the source document. Subelements can only be selected in the 3D view.
  4. Switch to the target document by clicking its tab in the Main view area.
  5. Invoke the tool as described above.

Inizia con SubShapeBinder vuoto

  1. Follow the instructions described under Same document above but without selecting geometry.
  2. An empty SubShapeBinder is created.
  3. Select the required geometry. Subelements can only be selected in the 3D view.
  4. In the Tree view drag and drop the selection onto the SubShapeBinder. If you have selected subelements their parent objects are highlighted in the Tree view, indicating the objects to be dragged.
  5. Optionally add more geometry in the same manner.
  6. To replace already referenced geometry hold down Ctrl during the drag and drop operation.


  • 2D offsetting is supported for some shape types, included planar faces, edges and wires. Because offsetting is a difficult operation for the software it does not always succeed. introduced in version 0.20
  • A SubShapeBinder that is not nested in a Body can be used as the Base Feature for a new Body.
  • The DatiSupport property contains the links to the referenced geometry. The property is read only by default, but can be changed by following the instructions described under Start with empty SubShapeBinder.
  • A SubShapeBinder created from a sketch can have an opposite "tool direction". For example a Pad created from the sketch may extend in the +Y direction, while a Pad, with the same properties, created from the SubShapeBinder extends in the -Y direction. Toggling the DatiReversed property (or checkbox) will solve this.


SubShapeBinder deriva da una Funzione Part (classe Part::Feature). Oltre alle proprietà elencate in Funzione Part, nell'editor delle proprietà sono disponibili le seguenti proprietà.



  • Dati (hidden)Support (XLinkSubList): supporto per la geometria.
  • DatiFuse (Bool): se è true fonde le forme solide legate.
  • DatiMake Face (Bool): se è true crea una faccia dalle polilinee connesse.
  • DatiClaim Children (PropertyBool): se è true richiama gli oggetti collegati come figli nella vista ad albero.
  • DatiRelative (Bool): se è true abiliterà il collegamento relativo degli oggetti secondari.
  • DatiBind Mode (Enumeration): modalità di legame, Synchronized, Frozen, Detached.
  • DatiPartial Load (Bool): se è true abiliterà il caricamento parziale degli oggetti.
  • Dati (hidden)Context (XLink): oggetto contenitore di questo oggetto raccoglitore.
  • Dati (hidden)_Version (Integer): versione di questo tipo di oggetto.
  • Dati (hidden)Shape (PartShape): Part TopoShape di questo oggetto.


  • Dati (hidden)Body (Matrix): matrice di unità di questo oggetto.


  • DatiOffset: 2D offset to apply. If Offset = 0, then no offset is applied. If Offset < 0, then the offset is applied inward. introduced in version 0.20
  • DatiOffset Join Type: Join method of offsetting non-tangent joints. The method can be Arcs, Tangent or Intersection. introduced in version 0.20
  • DatiOffset Fill (Bool): If true, a face is made between the new wire and the original wire. See also the DatiMake Face property. introduced in version 0.20
  • DatiOffset Open Result (Bool): Affects the way open wires are processed. If false, an open wire is made. If true, a closed wire is made from a double-sided offset, with rounds around open vertices. introduced in version 0.20
  • DatiOffset Intersection (Bool): Affects the way compounds are processed. If false, all children are processed independently. If true, and children are edges and wires, the children are offset in a collective manner. introduced in version 0.20