The tree view appears in the Model tab of the combo view, one of the most important panels in the interface; it shows all user defined objects that are part of a FreeCAD document. The tree view is a representation of the document's structure, and indicates what information is saved to disk.
The tree view showing various elements in the document.
Working with the tree view
By default, whenever a new object is created, it is added to the end of the list in the tree view. The tree view allows managing the objects to keep them organized; it permits creating groups, moving objects inside groups, moving groups inside other groups, renaming objects, copying objects, deleting objects, and other operations in the context menu (right click) which depend on the currently selected object and the currently active workbench.
Many operations create objects that are dependent on a previously existing object. In this case, the tree view shows this relationship by absorbing the older object inside the new object. Expanding and collapsing the objects in the tree view shows the parametric history of that object. Objects that are deeper inside others are older, while objects that are outside are newer, and are derived from the older objects. By modifying the interior objects, the parametric operations propagate all the way to the top, generating a new result.
The topmost object is created by doing parametric operations on objects which themselves were created by previous operations. Expanding the tree many levels reveals the original elements that were used to create the partial solids.
These allow working with various documents, but are disabled if no document is present.
Once a new document has been created the following become active:
In addition, Link actions are available.
Selecting the document
If you select the active document and right click, in addition to Expression actions and Link actions, the following commands appear:
- Show hidden items: if active, the tree view will show hidden items.
- Search: shows an input field to search objects inside the selected document.
- Close document: closes the selected document.
- Skip recomputes: if active, the document's objects will not recompute automatically.
- Allow partial recomputes: if active, the document will allow recompute of only some objects.
- Mark to recompute: marks all objects of the document as touched, and ready for recompute.
- Create group: creates a group in the selected document.
Once objects are added to the document right clicking them will show additional commands. These depend on the number of selected objects, their type and also on the active workbench. In most cases and with most workbenches (except the Start Workbench) the following commands are then available:
- Appearance: launches a dialog to change the visual properties of the whole object.
- Random color: assigns a random color to the object.
- Cut: disabled.
- Copy: copies an object into memory.
- Paste: pastes the copied object into the document; the copy is added to the end of the tree view.
- Delete: removes the object from the document.
- Hide item: if active, the selected object will be set as hidden.
- Add dependent objects to selection: all dependent objects will be added to the selection. This way one can see the dependencies and e.g. delete all dependent objects at once. This option is only available if one of the selected objects has links. introduced in version 0.20
- Mark to recompute: marks the selected object as touched, and ready for recompute.
- Recompute object: recomputes the selected object.
- Rename: starts editing the label of the selected object, not the name which is read-only. This option is only available if a single object is selected.
- Edit: activates the edit mode of the object.
- Transform: launches the transform widget to move or rotate the object.
- Attachment editor: launches a dialog to attach the object to one or more other objects.
- Set colors: sets the color of selected faces of the object.
- Toggle visibility: makes the object visible or invisible in the 3D view.
- Show selection: makes the selected object visible.
- Hide selection: makes the selected object invisible.
- Toggle selectability: toggles the selectability of the object in the 3D view.
- Select all instances: selects all instances of this object in the tree view.
- Send to Python Console: creates a variable in the Python console referencing the object
One or more smaller overlay icons can be displayed on top of an object's default icon in the tree view. The available overlay icons and their meaning are listed below. introduced in version 0.19
This indicates that the object has to be recomputed, due to changes made to the model or because the user marked the object in the tree view context menu to be recomputed. In most cases recomputes are triggered automatically, but sometimes they are delayed for performance reasons.
This indicates the so called Tip of a body. It is usually the last feature in a PartDesign Body and represents the whole body to the world outside of the body, e.g. when the body is exported or used in Part boolean operations. The tip can be changed by the user.
This is typically shown for sketches, geometric primitives, such as box, cylinder, etc. and Datum geometry. It indicates that the object is not attached to anything. It has no Attachment Offset and gets its position and alignment solely from its Placement property.
There is a Basic Attachment Tutorial explaining how to handle such objects.
This indicates that the object has an error that needs to be fixed. After recomputing the whole document a tooltip describing the error is shown when you hover the mouse over the object in the tree view. Note: All other objects depending on an object in such an error state will not be properly recomputed, thus they may still show some old state.