Creating Annotations in a 2D Layout for 3D Design Context

• 2D annotations
• associative 3D annotations
• associative hybrid annotations between 2D and 3D elements

As annotation commands work as in the Interactive Drafting workbench, the tasks included in the Annotations chapter provide links to the Interactive Drafting User's Guide. However, there are a few particularities about creating annotations in 2D Layout for 3D Design, as opposed to doing so in Drafting, which you will learn in this section.

In this section, you will learn about:

• Selecting elements to annotate
• Annotations in 2D Layout for 3D Design
  • Available commands
  • General behavior
  • Specific behaviors
  • Behavior of annotations with positional or orientation link
• Before you begin creating annotations in 2D Layout for 3D Design

Selecting elements to annotate

Annotation commands provide a visual feedback indicating whether it is possible to create annotations on a given element.

However, you should be aware of the following rule: in a given part layout, it is impossible to create an annotation which is associative in orientation or position to another part, as no link can be created between a part and another one. You can only create associative annotations within a single part layout. For example, in Part.1, it is not possible to store an annotation with a positional or orientation link to an element of Part.2.

When selecting elements to annotate, remember the following points:

• Annotations can be created in any view, even a non-active one.
• After starting an annotation command, the view in which you select the first element is the view of creation (that is the view where the annotation will be created).
• You can always select an element belonging to the view content.
• Once you have selected the first element, you can only select the other elements in the view of creation.
• You cannot select as the first element a 2D background element.
• You can select an element which belongs to the 3D background of a part layout only if this element belongs to the current layout.

Annotation behavior in 2D Layout for 3D Design

Available commands

You can create the following types of annotations: text, balloon, datum feature, datum target, geometrical tolerance, roughness symbol, welding symbol and table.

Note that in order to be consistent with the way commands have been grouped in toolbars and sub-toolbars, datum targets and geometrical tolerances are documented in the Dimensioning chapter.

In addition, it is possible to add leaders, positional links and orientation links to existing annotations. Regarding positional/orientation links, some restrictions apply, which are detailed in Behavior of annotations with positional or orientation link below.

General behavior

You can create annotations:

• in the main view, in the background view, or in a 2D component view (on a layout detail sheet).
• in any visible design view (projection view, auxiliary view, section view/cut) or isometric view of the current sheet, whether or not it is the active view.

To do so, you need to select (and not just point to) an element of the view in which you want to create the annotation.

Specific behaviors

Welding symbols

In the Drafting workbench, welding symbol leaders are positioned associatively to the intersection of two reference elements. As only one element can be selected in 2D Layout for 3D Design, the leader is simply positioned at the indicated position.

Text with attribute link

In 2D Layout for 3D Design, you can create the same attribute links as in the Drafting workbench.

The update mechanism is the same as in Drafting: if the referenced parameter is located in the same document, the text is automatically updated each time the parameter value is modified. But if the referenced parameter belongs to another document, you need to update the attribute link manually using the Local Update command available on the layout, sheet or view contextual menu.

Adding a leader to an existing annotation

You can add a leader to an existing annotation. However, you cannot select any kind of geometry. The leader is associative if you respect the rules detailed in Behavior of annotations with positional or orientation link below. If not, the leader is positioned at the indicated position.

Adding a positional or orientation link to an existing annotation

You can add a positional or orientation link to an existing annotation. However, you cannot select any kind of geometry. The link is created if you respect the rules detailed in Behavior of annotations with positional or orientation link below.

Updating a positional or orientation link when the reference element is modified

When the reference element for a positional or orientation link is modified, the way the link is updated depends on where the reference element is located:

Behavior of annotations with positional or orientation link

When creating annotations with positional or orientation link, there are two behaviors, depending on where you create the annotation.

If you create annotations in the main/background view or in a 2D component view

If you create annotations directly in the main view, in the background view, or in a 2D component view (on a layout detail sheet), no specific position in 3D space is defined. In this case, annotations are created exactly in the same context as in the Drafting workbench. Only view content elements may be selected. Therefore, annotation creation and edition commands behave exactly as in Drafting.

If you create annotations in a design/isometric view

If you create annotations in a design view or isometric view, a specific position in 3D space is defined. In this case, annotation creation and edition commands behave somewhat differently than in Drafting. Indeed, some restrictions apply regarding whether or not the annotation will be created with a positional/orientation link, as detailed below.

When editing a part layout outside the context of an assembly:

Only elements belonging to the same part or its associated layout are visible in a design/isometric view (including its background).

The table below sums up whether or not the annotation will be created with a positional/orientation link, depending on where the selected element is located and on what type of element you select:

When editing a part layout in the context of an assembly:

Elements belonging to the same part or its associated layout, as well as all elements belonging to any other part or product of the assembly, are visible in a design/isometric view (including its background).

However, remember that in a given part layout, it is impossible to create an annotation which is associative in orientation or position to another part, as no link can be created between a part and another one.

The table below sums up whether or not the annotation will be created with a positional/orientation link, depending on where the selected element is located and on what type of element you select:

Before you begin creating annotations in 2D Layout for 3D Design

Before you begin creating annotations in 2D Layout for 3D Design, make sure you are familiar with:

• The Tools toolbar and the Tools Palette.
• SmartPick, an easy-to-use tool designed to assist you when creating annotations. For more information, refer to the SmartPick task in the Sketcher User's Guide.
• Multi-selection. For more information, refer to the Selecting Objects chapter in the Infrastructure User's Guide.