Part and PartDesign/it

Descrizione
Ci sono state molte discussioni nel corso degli anni sulle differenze e le ramificazioni dell'uso degli ambienti Part e  PartDesign.

È una buona idea usare l'uno o l'altro finché l'utente non è a suo agio con uno, poi impara l'altro. È anche tipicamente raccomandato che i nuovi utenti non li confondano finché non hanno capito le differenze.

Parliamo di queste differenze.

Concetti dell'ambiente Part
L'ambiente Part è essenzialmente un modellatore di Geometrie solide. L'operatore combina varie primitive per finire con una rappresentazione della forma desiderata. (In effetti, l'ambiente Part va un passo oltre le primitive e permette all'operatore di usare un'operazione di schizzo+estrusione (o schizzo+rivoluzione, loft, sweep...) per creare anche forme casuali). Quando ogni primitiva o forma viene creata, non ha alcuna relazione con gli altri oggetti creati (tranne gli schizzi e i loro allegati), è un singolo solido isolato.



Questa condizione rimane tale fino a quando l'operatore usa delle operazioni per combinarli (tipicamente un booleano che li aggiunge o li sottrae). Ogni solido di partenza rimane accessibile separatamente e l'operazione crea un nuovo oggetto.

The take away is the single solitary solid bit and the combining them bit.

PartDesign Workbench Concepts
In the PartDesign Workbench the Body object is constructed directly as a single solitary cumulative solid.

The 1st step in a body must be a block of material, either from an additive primitive or an extrusion from a sketch, or an imported shape (then called Base Feature).

This initial block of material will be changed sequentially until the desired final shape (solid) is obtained.

It is cumulative in the sense that each operation adds or removes material.

By default, the "tip" of the body - unless there is a voluntary change in the visualization of a particular feature - is the last operation performed on the body. This is the current and visible state of the body, ready to be changed again by new feature.

Any function under the body represents the cumulative shape of the solid from the 1st feature to the feature considered.

So to have the complete solid, on the one hand the Tip feature must be the last stage of the construction of this solid, and on the other hand it is the body which must be selected and not a stage of its construction.

This will make it possible, in the event of a modification, to always have the last version of the solid represented.

Note and additions : At each time of the construction, the last function used is the "Tip", which can be defined too as "active stage in the construction of the object" or "stage preceding the next action in the construction of the object". When the object's drawing is complete, Tip is naturally the last stage or feature of the construction. But if desired, in case of forgetting, any feature of the construction can be provisionally declared as Tip: it then becomes the step preceding the next action in the construction of the object, which means that new feature(s) can be inserted anywhere in the construction, on condition not to create any incompatible with the suite.

When everything is finished, you have to redeclare the last feature as Tip, which corresponds to the finished object.



This image shows a Body. It is a cumulative solid that consists of a padded sketch and a cone primitive. This is a single solid.

If Tip on Pad, the pad can exist separately, but if Tip on Cone, the cone cannot exist separately (Tip on cone = pad + cone).

(Another thing mentioned often is a Body MUST be a single contiguous solid. This means all geometry created by a feature in the Body must touch it's predecessor.)

The Ramifications
Although not recommended for newcomers, it is possible to combine tools from Part WB and PartDesign WB, provided you know what you are doing. For example :

People get caught when they attempt to use some feature under the Body (rather than the Body itself) as one selection of a Part Workbench Boolean operation. This is a problem, because the selected feature does not represent THE complete solid.

In a sense, from a Part Workbench standpoint, the Body represents another primitive. So, using a Body (remember it is a proxy for the tip) and a Part Workbench object to do a Boolean is valid. But the resulting object is a Part WWorkbench object. And, thus PartDesign Workbench tools can't be used on it any longer.

And, it can get even more complicated. If you create a new Body and drag the result from the previous paragraph into it, a BaseObject is created. And you can go off an use the PartDesign Workbench tools on it.

The Caveats
There is a caveat with the Tip and it's representation of the single solid in the Body. If the tip is a subtractive feature and is used in a dress up operation, for instance a Mirror, the Mirror is operating on the underlying feature (a pocket for example). Thus the cumulative solid is not mirrored, but the subtractive feature is. The result of this must create a single solid.

In this example, a mirror of the tip (which is the pocket of the slot) around any of the base planes, or even a face of the solid will not produce a mirrored solid of the entire model. (In fact, it will produce a Mirrored feature in the tree that is essentially empty.)



In this example, a mirror of the tip (which is the pocket of the slot) is performed around the datum plane and produces a mirrored slot:



See the PartDesign Mirrored tool wiki page for more information.

Comparison
You can see below the same example built with each of the two workbenches. Of course, there are always several possible construction timelines with each workbench.

Compare the construction trees in the two workbenches as well as their organization and reading timeline :

Conclusion
Part and PartDesign workbenches can be used together with some care, creating quite complex models. Top