3D Shape Infrastructure | ||
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External Reference
- Keep link with selected object
- Maintains the links between external references,
(copied elements and imported elements), and their origins when you are
editing these elements.
This check box is used for editing 3D shapes included in assemblies. For more about designing 3D shapes in assembly context, see the Assembly Design User's Guide. To cut the link between external references and their origin, you need to use the Isolate command.
By default, this check box is cleared. - Show newly created external references
- Makes all external references you create from the
moment the option is on, are visible in the work area. The option does
not affect external references created before the check box was selected.
By default, this check box is cleared.
- Confirm when creating a link with selected object
- Warns if links are created
when you are pasting or importing elements from a separate 3D shape.
When Keep link with selected object check box is cleared, Confirm when creating a link with selected object remains available (can be selected or not). As some commands override the keep link with selected object status, a confirmation window is displayed.
By default, this check box is cleared. - Restrict external selection with link to published elements
- Permits only published
elements to be selected as external geometry. This restricts and therefore
controls the selections that can be made when selecting elements belonging
to a different 3D shape.
If Keep link with selected object is not cleared, this option has no effect.
By default, this check box is cleared. - Display relation status at representation level
- Displays the relation status at the representation level. If you select this check box, any one of the following masks appears on the representation node depending on the relation status:
Mask Description 
Indicates that the pointed object is not loaded in the session and the pointed object is not synchronized. 
Indicates that the pointed object is loaded in the session, but the pointed object is not synchronized. 
Indicates that the pointed object is deleted. 
Indicates that the pointed object is replaced by another version. By default, this check box is cleared. - Display relation status only on imported published elements
Views the relation status only on imported published elements.
By default, this check box is cleared.- Launch Replace Viewer during synchronization process
- Lets you contribute to the external reference
synchronization processes.
If selected, the Replace Viewer dialog box can appear during
interactive synchronization launched via commands such as Edit Links.
Additionally, the Replace Viewer dialog box will appear under
certain conditions: You can chose when the Replace Viewer dialog
box opens. By default, this check box is selected.
- Launch the Replace Viewer not always but only when really needed
- Launches the Replace Viewer only when the synchronization cannot solve issues
logically and therefore requires manual control. By default, this check box is selected.
Update
- Manual update
- Updates the feature when it is modified. The root is not updated. By default, this option is cleared.
- Automatic update
-
The root feature is automatically updated. By default, this option is selected.
- Stop Update on first error
- Stops the update process as soon as the app
finds an error when building the geometry. By default, this check box is cleared.
- Redraw updated elements during the update process
- Redraws the updates elements during the update process. By default, this check box is cleared.
- Synchronize all external references when updating the 3D shape
- Synchronizes all external references while updating the 3D shape, from which they are created. By default, this check box is cleared.
- Update dependencies when updating all
- Updates all the dependent constraints and shape representations in an assembly when you update the 3D shape. By default, this check box is cleared.
Delete Operation
- Display the Delete dialog box
- Displays the dialog box that lets you apply filters for deletion (see "Deleting
Features" in the Part Design Users Guide). By default, this option is selected.
- Delete exclusive parents
- Deletes the parents of the features you
are deleting. The parents will be deleted only if they are exclusive, in
other words, if they are not shared by other features. Conversely, if they
are shared by other features they will not be deleted.
When this setting is active, the option is selected in the Delete dialog box. Even if the option is selected in the Delete dialog box, you can uncheck it if you want to. If Display the Delete dialog box is cleared, this setting has no effect. For more information, see Deleting Features in the Part Design Users Guide.
By default, this option is cleared.
Replace
- Do replace only for elements situated after the In Work Object
- Replaces only the features located below the current feature and in the same branch. Ensure that at least one feature located below the current feature uses the feature you want to replace; otherwise, a warning message appears. This option is available only for the bodies and the ordered geometric sets, not for the solid bodies. By default, this check box is cleared.