Parte
Parte |
Posizione nel menu |
---|
Nessuno |
Ambiente |
Tutti |
Avvio veloce |
Nessuno |
Introdotto nella versione |
0.17 |
Vedere anche |
Gruppo, Corpo |
Descrizione
Una Parte (internamente chiamata App Part) è un contenitore per scopi generali che contiene un gruppo di oggetti in modo che essi possano essere spostati in blocco come una singola unità nella vissta 3D.
L'elemento Parte Standard è stato sviluppato per essere l'elemento di base per creare assemblaggi meccanici. In particolare, ha lo scopo di disporre oggetti che hanno una forma topologica, come le primitive di Part, i corpi di PartDesign, e altre funzioni di Part. Std Part fornisce un oggetto Origine con assi X, Y e Z locali e piani standard; questa origine viene utilizzata come riferimento per posizionare e collegare quegli altri oggetti. Inoltre, le parti standard possono essere nidificate all'interno di altre parti standard per creare un grande assieme da sottoassiemi più piccoli.
Sebbene sia destinato principalmente a corpi solidi, Parte standard può essere utilizzato per gestire qualsiasi oggetto che abbia una proprietà Posizionamento, quindi può anche contenere funzioni Mesh, schizzi e altri oggetti derivati dalla classe App GeoFeature.
Non confondere il Corpo di PartDesign con la Parte standard. Il primo è un oggetto specifico utilizzato in PartDesign, destinato a modellare un singolo solido contiguo mediante le funzioni di PartDesign. Invece, la Parte non viene utilizzata per la modellazione, ma solo per disporre diversi oggetti nello spazio, per creare degli assemblaggi.
Lo strumento Std Part non è definito da un particolare ambiente di lavoro, ma dal sistema base; di conseguenza lo si trova nella barra degli strumenti struttura, che è disponibile in tutti gli ambienti di lavoro. Per raggruppare gli oggetti arbitrariamente senza considerare la loro posizione, utilizzare Gruppo; questo oggetto non influenza i posizionamenti degli elementi che contiene, è essenzialmente solo una cartella che viene utilizzata per mantenere organizzata la vista ad albero.
A sinistra: elementi all'interno di una Parte Std nella vista ad albero. A destra: oggetti posizionati nello spazio, riferiti all'Origine della Parte Std.
Utilizzo
- Premere il pulsante Parte. Viene creata una parte vuota che diventa automaticamente attiva.
- Per aggiungere oggetti a una parte, trascinarli e rilasciarli sulla parte nella vista ad albero.
- Per rimuovere oggetti da una parte, trascinarli fuori dalla parte e sull'etichetta del documento nella parte superiore della vista ad albero.
Note
- A partire dalla v0.19, un dato oggetto può appartenere solo ad una singola Parte.
- Fare doppio clic sulla Parte nella vista ad albero o aprire il menu contestuale (tasto destro del mouse) e selezionare Attiva/disattiva la parte per attivare o disattivare la Parte. Se un'altra Parte è attiva, sarà disattivata. Vedere Stato attivo per maggiori informazioni.
Limitazioni
- Al momento, i metodi Snap di Draft non funzionano sui contenitori di Parti selezionati né sugli oggetti al loro interno.
- Una Parte standard non ha una forma topologica, quindi operazioni 3D come le operazioni booleane non possono essere utilizzate su una parte. Ad esempio, non è possibile selezionare due parti ed eseguire una Unione o un Taglio con esse.
- Queste operazioni booleane funzionano solo sugli oggetti contenuti fintanto che sono derivati da Part Feature e hanno una forma topologica.
Proprietà
Una Std Part è internamente chiamata App Part (App::Part
class), e deriva da un App GeoFeature (App::GeoFeature
class), quindi condivide la maggior parte delle proprietà di quest'ultimo.
In addition to the properties described in App GeoFeature, the App Part class has some properties that help it manage information in the context of an assembly, for example, DatiType, DatiId, DatiLicense, DatiLicenseURL, DatiColor, and DatiGroup.
These are the properties available in the property editor. Hidden properties can be shown by using the Show all command in the context menu of the property editor.
Data
Base
- DatiId: ID (Numero di parte) dell'elemento. Questo campo è facoltativo.
- DatiLicense: la licenza con cui viene rilasciata la parte.
- DatiLicense URL: l'indirizzo Web in cui è possibile trovare i termini della licenza.
- DatiPlacement: specifica l'orientamento e la posizione della parte nello spazio 3D. Vedere Posizionamento.
- DatiLabel: l'etichetta è il nome dato all'operazione. Questo nome può essere cambiato a piacimento.
- DatiGroup: elenca gli oggetti riferiti.
Hidden properties Data
- DatiMaterial (
Map
): map with material properties. By default, it is empty{}
. - DatiMeta (
Map
): map with additional meta information. By default, it is empty{}
. - DatiUid (
UUID
): the universally unique identifier (UUID) (128-bit number) of the object. This is assigned at creation time. - DatiLabel2 (
String
): a longer, user editable description of this object, it is an arbitrary UTF8 string that may include newlines. By default, it is an empty string""
. - DatiExpression Engine (
ExpressionEngine
): a list of expressions. By default, it is empty[]
. - DatiVisibility (
Bool
): whether to display the object or not. - DatiOrigin (
Link
): the App Origin object that is the positional reference for all elements listed in DatiGroup. - Dati_ Group Touched (
Bool
): whether the group is touched or not.
View
The App Part only has the five properties of the basic App FeaturePython, and it does not have hidden properties.
Base
- VistaDisplay Mode (
Enumeration
):Group
. - VistaOn Top When Selected (
Enumeration
):Disabled
(default),Enabled
,Object
,Element
. - VistaSelection Style (
Enumeration
):Shape
(default),BoundBox
. If the option isShape
, the entire shape (vertices, edges, and faces) will be highlighted in the 3D view; if it isBoundBox
only the bounding box will be highlighted. - VistaShow In Tree (
Bool
): if it istrue
, the object appears in the tree view. Otherwise, it is set as invisible. - VistaVisibility (
Bool
): if it istrue
, the object appears in the 3D view; otherwise it is invisible. By default this property can be toggled on and off by pressing the Space bar in the keyboard.
Concetto di assemblaggio
The Std Part is intended to be the basic building block to create assemblies. Unlike a PartDesign Body, an assembly is meant to be a collection of separate, distinguishable elements which are connected in some way in the physical world, for example, through pressure, screws, or glue.
Examples that could be Parts:
- A wooden table that consists of individual wooden pieces (legs, top), which are put together by glue or metal screws.
- A ball bearing that is composed of multiple steel balls, an inner ring, a retainer, a seal, and an outer ring.
- An assembly of a screw with a washer, and a matching nut.
Left: three individual contiguous solids, each of them modelled by a PartDesign Body. Right: the individual Bodies put together inside a Std Part to create an assembly.
In general terms, when importing a STEP file into the program, the main assembly and its sub-assemblies will be imported as Part containers, each of them containing a simple Part Feature.
Detailed explanation
Stato attivo
An open document can contain multiple Parts. An active Part will be displayed in the tree view with the background color specified by the Active container value in the preferences editor (by default, light blue). An active part will also be shown in bold text.
To activate or de-activate a Part:
- Double click on it on the tree view, or
- Open the context menu (right click) and select Toggle active part.
Notes:
- The active status of Parts was developed in v0.17 in parallel with the active status of PartDesign Bodies; however, as of v0.19 this status does not serve a real purpose for Parts.
- Even when a Part is active, newly created objects are not placed inside of it automatically. In this case, simply drag these new objects, and drop them onto the desired Part.
- Only a single Part can be active at a time.
Document with two Std Parts, of which the second one is active.
Origine
The Origin consists of the three standard axes (X, Y, Z) and three standard planes (XY, XZ and YZ). Sketches and other objects can be attached to these elements when creating them.
Left: Part Origin in the tree view. Right: representation of the Origin elements in the 3D view.
Note: the Origin is an App Origin object (App::Origin
class), while the axes and planes are objects of type App::Line
and App::Plane
respectively. Each of these elements can be hidden and unhidden individually with the Space bar; this is useful to choose the correct reference when creating other objects.
Note 2: all elements inside the Part are referenced to the Part's Origin which means that the Part can be moved and rotated in reference to the global coordinate system without affecting the placement of the elements inside.
Gestione della visibilità
The Part's visibility supersedes the visibility of any object it contains. If the Part is hidden, the objects it contains will be hidden as well, even if their individual VistaVisibility property is set to true
. If the Part is visible, then each object's VistaVisibility determines whether the object is shown or not.
The visibility of the Std Part determines whether the objects grouped under it are shown in the 3D view or not. Left: the Part is hidden, so none of the objects will be shown in the 3D view. Right: the Part is visible, so each object controls its own visibility.
Inheritance
A Std Part is formally an instance of the class App::Part
, whose parent is the basic App GeoFeature (App::GeoFeature
class), and is augmented with an Origin extension.
Simplified diagram of the relationships between the core objects in the program. The App::Part
class is a simple container that has a position in 3D space, and has an Origin to control the placement of the objects grouped under it.
Scripting
See also: FreeCAD Scripting Basics, and scripted objects.
See Part Feature for the general information on adding objects to the document.
A Std Part (App Part) is created with the addObject()
method of the document. Once a Part exists, other objects can be added to it with the addObject()
or addObjects()
methods of this Part.
import FreeCAD as App
doc = App.newDocument()
obj = App.ActiveDocument.addObject("App::Part", "Part")
bod1 = App.ActiveDocument.addObject("PartDesign::Body", "Body")
bod2 = App.ActiveDocument.addObject("Part::Box", "Box")
obj.addObjects([bod1, bod2])
App.ActiveDocument.recompute()
A Part is a container for other objects, so it doesn't have its own Shape (Part TopoShape). However, in expressions or in the Spreadsheet Workbench, it is useful to get the compound shape of all objects contained inside the Part. This can be accomplished by using the _shape
pseudo-property, which can then be used to extract other attributes.
=Part._shape.Edges[0].Length
- File: New, Open, Close, Close All, Save, Save As, Save a Copy, Save All, Revert, Import, Export,Merge project, Project information, Print, Print preview, Export PDF, Recent files, Exit
- Edit: Undo, Redo, Cut, Copy, Paste, Duplicate selection, Refresh, Box selection, Box element selection, Select All, Delete, Send to Python Console, Placement, Transform, Alignment, Toggle Edit mode, Edit mode, Preferences
- View:
- Miscellaneous: Create new view, Orthographic view, Perspective view, Fullscreen, Bounding box, Toggle axis cross, Clipping plane, Texture mapping, Toggle navigation/Edit mode, Appearance, Random color, Workbench, Status bar
- Standard views: Fit all, Fit selection, Isometric, Dimetric, Trimetric, Home, Front, Top, Right, Rear, Bottom, Left, Rotate Left, Rotate Right
- Freeze display: Save views, Load views, Freeze view, Clear views
- Draw style: As is, Points, Wireframe, Hidden line, No shading, Shaded, Flat lines
- Stereo: Stereo red/cyan, Stereo quad buffer, Stereo Interleaved Rows, Stereo Interleaved Columns, Stereo Off, Issue camera position
- Zoom: Zoom In, Zoom Out, Box zoom
- Document window: Docked, Undocked, Fullscreen
- Visibility: Toggle visibility, Show selection, Hide selection, Select visible objects, Toggle all objects, Show all objects, Hide all objects, Toggle selectability, Toggle measurement, Clear measurement
- Toolbars: File, Edit, Clipboard, Workbench, Macro, View, Structure, Help
- Panels: Tree view, Property view, Selection view, Tasks, Python console, DAG view, Model, Report view
- Link navigation: Go to linked object, Go to the deepest linked object, Select all links
- Tree view actions: Sync view, Sync selection, Sync placement, Pre-selection, Record selection, Single document, Multi document, Collapse/Expand, Initiate dragging, Go to selection, Selection Back, Selection Forward
- Tools: Edit parameters, Save image, Load image, Scene inspector, Dependency graph, Project utility, Measure distance, Add text document, View turntable, Units calculator, Customize, Addon manager
- Macro: Macro recording, Macros, Recent macros, Execute macro, Attach to remote debugger, Debug macro, Stop debugging, Step over, Step into, Toggle breakpoint
- Help: Help, FreeCAD Website, Donate, Users documentation, Python scripting documentation, Automatic Python modules documentation, FreeCAD Forum, FreeCAD FAQ, Report a bug, About FreeCAD, What's This
- Structure tools: Part, Group
- Helper tools: Create body, Create sketch, Edit sketch, Map sketch to face
- Modeling tools
- Datum tools: Create a datum point, Create a datum line, Create a datum plane, Create a local coordinate system, Create a shape binder, Create a sub-object(s) shape binder, Create a clone
- Additive tools: Pad, Revolution, Additive loft, Additive pipe, Additive helix, Additive box, Additive cylinder, Additive sphere, Additive cone, Additive ellipsoid, Additive torus, Additive prism, Additive wedge
- Subtractive tools: Pocket, Hole, Groove, Subtractive loft, Subtractive pipe, Subtractive helix, Subtractive box, Subtractive cylinder, Subtractive sphere, Subtractive cone, Subtractive ellipsoid, Subtractive torus, Subtractive prism, Subtractive wedge
- Transformation tools: Mirrored, Linear Pattern, Polar Pattern, Create MultiTransform, Scaled
- Dress-up tools: Fillet, Chamfer, Draft, Thickness
- Boolean: Boolean operation
- Extras: Migrate, Sprocket, Involute gear, Shaft design wizard
- Context menu: Set tip, Move object to other body, Move object after other object, Appearance, Color per face
- Getting started
- Installation: Download, Windows, Linux, Mac, Additional components, Docker, AppImage, Ubuntu Snap
- Basics: About FreeCAD, Interface, Mouse navigation, Selection methods, Object name, Preferences, Workbenches, Document structure, Properties, Help FreeCAD, Donate
- Help: Tutorials, Video tutorials
- Workbenches: Std Base, Arch, Assembly, CAM, Draft, FEM, Inspection, Mesh, OpenSCAD, Part, PartDesign, Points, Reverse Engineering, Robot, Sketcher, Spreadsheet, Surface, TechDraw, Test Framework
- Hubs: User hub, Power users hub, Developer hub