Feature editing/it

Introduzione
This page explains the way the PartDesign Workbench is intended to be used starting with FreeCAD 0.17.

Mentre l'ambiente Part e altri ambienti di FreeCAD costruiscono i modelli combinando insieme delle forme, l'ambiente PartDesign usa le. Una feature è un'operazione che modifica la forma di un modello.

Metodologia delle funzioni editabili
La prima funzione è chiamata comunemente funzione di base. Quando si aggiungono ulteriori funzioni al modello, ogni funzione prende la forma precedente e vi aggiunge o rimuove del materiale, creando delle dipendenze lineari tra una funzione e quella successiva. In effetti, questa metodologia simula un comune processo di produzione: un blocco viene tagliato su un lato, quindi su un altro lato, vengono aggiunti dei fori, poi dei raccordi, ecc.

Tutte le funzioni sono elencate in sequenza nell'albero del modello e possono essere modificate in qualsiasi momento. L'ultima funzione che è situata nella parte inferiore rappresenta la parte finale.

Le funzioni possono essere ordinate in diverse categorie:


 * Basata su profili: queste funzioni partono da un profilo per definire la forma dell materiale da aggiungere o rimuovere. Il profilo può essere costituito da uno schizzo, una faccia planare sulla geometria esistente (il profilo viene estratto dai suoi bordi), un oggetto ShapeBinder o un oggetto Draft che è stato incluso nel corpo attivo.


 * Additiva: aggiunge del materiale al modello esistente. Le funzioni additive mostrano delle icone gialle.


 * Sottrattiva: rimuove la materia dal modello esistente. Le funzioni sottrattive mostrano delle icone rosse e blu.


 * Basata su primitive: basata su primitive geometriche (cubo, cilindro, cono, toro ...). Possono essere additive o sottrattive.


 * Funzioni di trasformazione: applicano una trasformazione a delle funzioni esistenti (riflessione, schiera lineare, schiera polare, multitrasformazione).


 * Dress-up: features that apply a treatment to edges or faces, such as fillets/rounds, chamfers and drafts.


 * Procedural: can be said of features that are not based on sketches, like the transformation and dress-up features.

Body
Working in PartDesign requires first creating a Body. The PartDesign Body is a container that groups a sequence of features forming a single contiguous solid.



What is a single contiguous solid? It is an object like a casting or something machined from a single block of metal. If the object involves nails, screws, glue or welding, it is not a single contiguous solid. As a practical example, a wooden chair would be made of multiple bodies, with one for each of its sub-components (legs, slats, seat, etc).

Multiple bodies can be created in a FreeCAD document; they can also be combined to form a single contiguous solid.

Only one body can be active in a document. The active body gets the new created features. A body can be activated or deactivated by double clicking on it. An activated body is highlighted in light blue. The highlighting color can be set in the preferences under Display/Colors/Active container since version 0.18.

When a model requires multiple bodies, like the previous wooden chair example, the general purpose Part container can be used to group them and move the whole as a unit.

Body visibility management
A body will present by default its most recent feature to the outside. This feature is defined by default as the tip. A good analogy is the expression the tip of the iceberg: only the tip is visible above the water, most of the iceberg's mass (the other features) is hidden. As a new feature is added to the body, visibility of the previous feature is turned off, and the new feature becomes the tip.

There can only be one feature visible at a time. It is possible to toggle the visibility of any feature in the body, by selecting it in the Model tree and pressing the spacebar, in effect going back in the history of the body.

Body Origin
The body has an Origin which consists of reference planes (XY, XZ, YZ) and axes (X, Y, Z) that can be used by sketches and features. Sketches can be attached to Origin planes, and they no longer need to be mapped to planar faces for features based on them to be added or subtracted from the model.

Moving and Reordering Objects
It is possible to temporarily redefine the tip to a feature in the middle of the Body tree to insert new objects (features, sketches or datum geometry). It is also possible to reorder features under a Body, or to move them to a different Body. Select the object and right-click to get a contextual menu that will offer both options. The operation may be prevented if the object has dependencies in the source Body, such as being attached to a face. To move a sketch to another Body, it should not contain links to external geometry.

Datum geometry
Datum geometry consists of custom planes, lines, points or externally linked shapes. They can be created for use as reference by sketches and features. There is a multitude of attachment possibilities for datums.

Cross-referencing
It is possible to cross-reference elements from a body in another body via datums. For example the datum shape binder allows to copy over faces from a body as reference in another one. This should make it easy to build a box with fitting cover in two different bodies. FreeCAD helps you to not accidentally link to other bodies and queries your intent.

Attachment
Object attachment is not a specific PartDesign tool, but rather a Part utility introduced in v0.17 that can be found in the Part menu. It is heavily used in the PartDesign workbench to attach sketches and reference geometry to the standard planes and axes of the Body. Very extensive ways of creating datum points, lines and planes are available. Optional attachment offset parameters make this tool very versatile.

More info can be found in the Attachment page.

Advice for creating stable models
The idea of parametric modeling implies that you can change the values of certain parameters and subsequent steps are changed according to the new values. However, when severe changes are made, the model can break due to the topological naming issue that is still unresolved in FreeCAD. Compared to previous FreeCAD versions, breakage can be minimized when you respect the following design principles:


 * Avoid as much as possible mapping sketches to faces of the model. Place your sketches on standard planes, or on custom datum planes. Sketches attached to planes are less at risk of being unexpectedly reattached to a different reference.
 * When creating datum geometry, do not base it on the part topology, base it on standard planes/axes and/or sketches.
 * Use a "master sketch". That is a preferably not too complicated sketch which contains basic geometric elements of your model. These elements can be referenced when modeling subsequent features. Such a master sketch will often be the first sketch in the Body but it doesn't have to be; in fact you don't even have to use it at all for anything else but being referenced.
 * If you inevitably have to reference an intermediate feature, e.g. the result of a thickness operation, use the first reference possible in the list of subsequent features where the referenced geometric element occurs. From FreeCAD 0.17 on you don't have to use the latest feature. If you take an early feature as reference, all changes to intermediate steps won't break your model. And again it is better to reference a sketch than edges and vertices of a solid.