Creating Imports

You can create imports. Using the Create Import command, you can have a better control of the destination of the import elements you create.

Before you begin: Activate the representation where the import is to be created.
See Also
About the Import Creation Command
  1. In the Tools section of the action bar, click Create Import .
    The Create Import dialog box appears.
    Important: The command is exclusive and allows preselection.
  2. In the Import box, select the object from which you want to create external and internal references.
    Note: The supported elements are:
    • wireframe and surface features
    • volumes
    • sketches
    • bodies
    • parameters (if they are set as visible in the Preferences)
    • solid functional sets (SFS)
    • functional specifications
    • functional sets.

    The last three elements are only available with the Functional Modeling Part apps.

    The name of the object appears in the Import box.

  3. In the Destination box, select the destination where import to be created will be aggregated.

    By default, the destination is the in work object.

  4. In the Position list, select the position of the import to be created, relative to the destination:
    • After: the element is positioned after the reference.
    • Before: the element is positioned before the reference.
    • Inside: the element is positioned inside the reference.
    The element will be imported in the place you selected.
    Notes:
    • The list only presents choices that are possible.
    • The default value is After (when the choice is possible).
  5. In the Result list, select the type of result you require after the duplication.
    Important: The list updates according to the type of feature you want to import.
    Note: Some features have more than one geometrical result. For instance, a sheet metal body can have a form result and a flat result.
  6. Select the type of associativity:
    • Not associative with the initial selected element: clear the Keep link option.
      Note: If the box is cleared, a datum feature without link is created.
      Important: If the box was initially selected and then cleared, it is possible that no object is created (because of multi-context cycle). In this case, no action is taken at this stage but an error message appears when validating.
    • Associative, including in position, (relevant to Assembly Design only): the Keep link and Keep context options are selected.
      Important: By default, for associative imports, the associativity mode is in shape and position. Therefore the Keep context option is available only when Keep Link is selected.
    • Associative (in terms of geometrical shape but not in position): the Keep link option is activated.

    Important: By selecting the options, you can switch to an associative import, which is only associative in terms of shape but not in position.

  7. Click OK when satisfied.
    • The created imports are inserted in the tree.
    • The solid external references are created in a solid body or a body, according to the Enable hybrid Design check box in Me > Preferences > Common Preferences > Object Properties > 3D Shape > Infrastructure, 3D Shape Infrastructure area, 3D Shape Infrastructure area, Hybrid Design section.

Important:
  • For internal import, the default state of the feature pasted with the As Result with Link option is unfrozen. In this state, the copied geometry is synchronized with its source.
  • You can freeze imports. When elements are imported using multi-part links (external references) or using the Copy-Paste As result with link capability, the deactivation concerns the link, not the feature. As a consequence, the feature can still be selected. For more information about freezing links, refer to Part Design User’s Guide: Freezing Links.