|Part Design → Create body|
|Introduced in version|
|Std Part, feature editing|
A PartDesign Body is the base element to create solids shapes with the PartDesign Workbench. It can contain sketches, datums objects, and PartDesign features in order to produce a single contiguous solid.
The Body provides an Origin object which includes local X, Y, and Z axes, and planes. These elements can be used as references to attach sketches and primitive objects.
Since the Body is supposed to be a single contiguous solid, it can be moved entirely as a unit, without moving the individual features. Multiple bodies can be placed inside Std Parts in order to create assemblies.
Left: the tree view showing the features that sequentially produce the final shape of the object. Right: the final object visible in the 3D view.
How to use
If no previous solid is selected:
- Press the button. An empty Body is created and automatically becomes active.
- Now you can press to create a sketch in the Body that can be used with .
- Alternatively, add a primitive solid feature, for example, .
If a solid object is selected:
- Press the Part Workbench or imported from a Step file) that we want to modify further with PartDesign tools. button. A new body is created containing a single BaseFeature. This BaseFeature element is a simple reference to another object previously created or imported into the document. The BaseFeature can also be created by dragging that solid into an empty Body. This is done when we have a pre-existing solid (for example, created with the
- An existing Body cannot be selected when pressing DataBase Feature property. button. However, an existing Body can be used as the BaseFeature by adding that object to the
- If no Body currently exists, when is pressed on the PartDesign toolbar, a new Body will be automatically created.
- Double-click the Body in the tree view or open the context menu (right-click) and select Toggle active body to activate or deactivate the Body. If another Body is active, it will be deactivated.
- DataTip: the feature defined as "Tip". The Tip is usually the last feature created in the Body, although any of the previous features can also be set as the Tip. This indicates which is the final shape of the Body, which is displayed when ViewDisplay Mode Body is set to
- DataBase Feature: an external shape used as the first feature in the Body. It is usually set when dragging a solid object into an empty Body. If the first feature is created from a and a , or from a primitive solid, for example, an , then the BaseFeature is empty.
- DataGroup: a list with the feature objects inside the Body.
- DataPlacement: the position of the object in the 3D view. The placement is defined by a
Basepoint (vector), and a
Rotation(axis and angle). See Placement.
- ViewDisplay Mode Body: sets the display mode specifically for the Body with one of two types.
Through(default) exposes all objects inside the Body, that is, sketches, features, datum objects, etc. This mode allows visualizing partial operations done inside the Body, and thus it is the recommended mode when adding and editing features. Select the specific feature, and the set ViewVisibility to or press on the keyboard.
Tipexposes only the final shape of the Body, which is defined by the DataTip property. Everything else, including sketches, partial features, datums, etc., is not displayed, even if they are visible in the tree view. This mode is recommended when the Body does not need to be modified further, so a fixed shape is shown. This mode is also recommended when you wish to select the sub-elements (vertices, edges, and faces) of the final shape to use with other workbenches' tools.
Single contiguous solid
A PartDesign Body is intended to model a single contiguous solid. The meaning of "contiguous" is an element made in one piece, with no moving parts, or disconnected solids. Examples of contiguous solids are those that are manufactured from a single piece of raw material by a process of casting, cutting, or milling. For example, a nut, a washer, and a bolt can each be fabricated separately, so each can be modelled by a PartDesign Body. Objects that are created by welding two pieces can also be modelled by a single Body as long as the weld joint is solid and not intended to break apart.
Once these contiguous solids are put together in some type of arrangement, then they become an "assembly".
Left: three individual contiguous solids, each of them modelled by a PartDesign Body. Right: the individual Bodies put together in an assembly.
A PartDesign Body is intended to work by creating an initial solid, either from a Sketch or from a primitive shape, and then modifying it through "features" that add or remove material from the previous shape. For a full explanation go to feature editing.
A PartDesign Body will perform an automatic fusion of the solid elements inside of it. This means that the partial solids should be touching, and disconnected solids are not allowed.
Left: two individual solids that intersect each other. Right: a single PartDesign Body with two additive features; they are automatically fused together, so instead of intersecting, they form a single continuous solid.
Left: two disconnected solids; this isn't a valid PartDesign Body. Right: two touching solids; this results in a valid PartDesign Body. The newer feature should always contact or intersect the previous feature so that it is fused to it, and becomes a single contiguous solid.
An open document can contain multiple Bodies. To add a new feature to a specific Body, it needs to be made active. An active body 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 body will also be shown in bold text.
To activate or de-activate a Body:
- Double click on it on the tree view, or
- Open the context menu (right click) and select Toggle active body.
Activating a Body automatically switches to the PartDesign Workbench. Only a single Body can be active at a time.
The active Body can be defined from the Python console by using the
setActiveObject method of the
ActiveView. The first argument is the fixed string
"pdbody", and the second argument is the Body object itself.
import FreeCAD as App import FreeCADGui as Gui App.newDocument() obj = App.ActiveDocument.addObject("PartDesign::Body", "Body") Gui.ActiveDocument.ActiveView.setActiveObject("pdbody", obj)
The Origin consists of the three standard axes (X, Y, Z) and three standard planes (XY, XZ and YZ). Sketches can be attached to these planes, and planes along with axes can be used to create other datum (reference) geometry. All elements inside the Body are referenced to the Body's Origin; which means that the body can be moved and rotated in reference to the global coordinate system without affecting the placement of elements inside the body.
The base feature is by definition the first PartDesign feature created in the Body. But it is possible to use a solid shape, either imported or modelled in other workbenches, as a base feature to which sketches and other features can be added.
The tip is the feature that is exposed outside the Body. It is automatically set to the last feature at the bottom of the tree. But sometimes it can be useful to change it to an earlier feature in the Body tree, which in effect rolls back its history; then it is possible to add features that should have been added earlier. In the Body tree, the feature set to tip displays a green dot with a white down arrow in it.
For more details, see the Move Tip page.
The Body's visibility supersedes the visibility of any object it contains. If the Body is hidden, the objects it contains will be hidden as well, even if their visibility is set to true. Only one feature can be visible at a time. Selecting a hidden feature and pressing thewill make it visible, and automatically hide the previously visible feature.
Interaction with other workbenches
By default, objects underneath a Body are selectable, and this is of course required to edit and add features in PartDesign. But selecting a Body's features to create operations from other workbenches (like Part or Draft) is not advised, as the results may be unexpected; in all cases, an error labelled Links go out of the allowed scope will appear in the Report view.
Therefore, for interactions with other workbenches, only the Body itself should be selected from the Model tree. In cases where it is necessary to select specific topology on the Body (vertex, edge, face), then the Body's Display Mode Body view property can be switched from Through (default) to Tip. This property is accessible from the View panel. In Tip mode, access to the objects under the Body (features, datums, sketches) is disabled; everything but the tip feature will be hidden in the 3D view, no matter which object is set as visible.
Once operations in other workbenches are completed, do not forget to reset the Display Mode Body property to Through to be able to edit the Body.
Simplified diagram of the relationships between the core objects in the program. The
PartDesign::Body object is intended to build parametric 3D solids, and thus is derived from the basic
See Part Feature for the general information.
A PartDesign Body is created with the
addObject() method of the document. Once a body exists, features, like additive and subtractive primitives, can be added and attached to that body.
import FreeCAD as App doc = App.newDocument() obj = App.ActiveDocument.addObject('PartDesign::Body', 'Body') obj.Label = "Custom label" feature = App.ActiveDocument.addObject('PartDesign::AdditiveBox', 'Box') obj.addObject(feature) App.ActiveDocument.recompute()