About Creating Annotations in Assembly Context

Annotations between components of an assembly are created using engineering connection.

This page discusses:

See Also
Creating Annotations in Assembly Context

Selection of Elements

You can select elements which are located outside of annotation set while creating or modifying annotations and/or dimensions in the current annotation set.

Selection of elements located outside of the annotation set is possible during the following creation commands:

  • Annotations:
    • Text
    • Text with Leader
    • Table
    • Datum Feature
    • Datum Target
    • Geometrical Tolerance
    • Roughness Symbol
    • Welding Symbol
  • Dimensions:
    • Dimensions
    • Chained Dimensions
    • Cumulated Dimensions
    • Stacked Dimensions

Selection of elements located outside the annotation set is possible during the following modification commands:

  • Annotations:
    • Positional Link > Create, Positional Link > Replace
    • Orientation Link > Create, Orientation Link > Replace
  • Dimensions:
    • Re-route Dimension

You can select vertex point and edges of 3D geometry which belong to other representations to create annotations and dimensions.

You can select product instances to create annotation, in this case the annotation will be applied to whole product instance.

Depending on a dedicated option as explained in Assembly Context section selections are possible, see Administration:

  • Only under the active assembly root product
  • Only under the favorite context root
  • In the assembly

However, if the selected element is not under the active assembly root product or under the favorite context root, appropriate message appears.

Referenced Geometry

You can annotate geometry of the product coming from other representations in the same product structure.

You can create annotations referencing geometries located either inside or outside the annotation set but not both.

For example, an annotation which has a positional link on an element located inside the annotation set cannot have an orientation link on an element located outside the annotation set.

On the other hand, an annotation can have several leaders with positional links on elements located inside several representations other than the annotation set.

Engineering Connection

Annotation definition determines a functional or geometrical specification of the product. These definitions are stored inside the engineering connection and their presentations maintain a link from their representation to this engineering connection.

The creation of annotation definition is automatically performed only when the selection is outside the annotation set, when creating an annotation, adding a leader to any annotation, creating a dimension, or adding an associative positional link.

Thus, large amount of such annotation definition entities could be created in the database.

So, to avoid this, existing Engineering Connections are reused when an additional annotation is created referencing the same occurrence and having the same orientation and parent product.

This behavior holds true even if the existing Engineering Connection does not contain annotation definitions but other data, like assembly constraints, for example.

Note that a regular engineering connection is an engineering connection created between the child products of the active product.

You can delete the annotation definition by deleting its own engineering connection or by clicking Remove in the Engineering Connection Definition dialog box.

However, it does not delete its presentation and therefore the presentation remains isolated from its definition.

It means that there is no automatic deletion of the presentations when deleting a definition.

However, you can identify presentations with a broken relation by using the Links & Relations command.

When all the related links and relations are already resolved using Update or Links & Relations but the links are still missing:

  1. Right-click the annotation set node in the tree.
  2. Select Annotation Set.X object > Automatically reconnect FTA definition features .
This reroutes the FTA presentation annotation disconnected from its definition feature with the respective FTA definition feature, located inside the right engineering connection, which is selectively loaded in current product configuration.

Note: For more information about engineering connections, see the 3D Modeling: Mechanical Systems: Assembly Design User’s Guide.