|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: displays and sets the feature defined as "Tip".
- DataBase Feature: displays and sets the external shape used as base feature. It does not apply if a PartDesign feature is the base feature.
- DataGroup: lists the referenced objects inside the Body.
- ViewDisplay Mode Body: sets the display between two modes:
- Through (default) exposes everything inside the body (features, datums, sketches, etc.). It is the mode used in adding and editing features inside the body.
- Tip exposes only the shape of the Body itself according to the set tip; everything else including sketches is hidden from view and cannot be displayed. Practical use: "Tip" allows selection of edges and faces of the Body to create operations from other workbenches.
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 a Body:
- Double click on it, or
- Open the context menu (right click) and select Toggle active body.
Activating a Body automatically switches the interface to the PartDesign Workbench. Only a single Body can be active at a time.
The active Body can be defined from the Python console using the
setActiveObject method of the
import FreeCAD as App import FreeCADGui as Gui ... obj = App.ActiveDocument.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.
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()