Managing 3D Annotations in 3D XML Files

This task explains you how to manage 3D Annotations in 3D XML files:
 

Save

  • The Save as 3D XML capability is provided by File> Save as... or File> Save Management> Save as... For more information, please refer to Saving Documents in Other Formats in CATIA Infrastructure User's Guide.
  • The Save as 3D XML capability in batch mode is not provided.
  • To save 3D annotations in a 3D XML file, select the 3D annotation check box in Tools> Options> General> Compatibility> 3D XML.

  • The 3D annotation option is active for the Dynamic Tessellation and Static Tessellation geometry representation formats, selected in Tools> Options>  General> Compatibility> 3D XML, Geometry Representation area. The 3D annotations will be saved in 3D XML file for these geometry representations.

  • The XmlTessellation geometry representation format does not support saving of 3D annotations in a 3D XML file. The 3D annotations option will be inactive in this case.

  • 3D annotations of CATParts are taken into account.
  • 3D annotations created at a product and process level are also taken into account
  • Note that Datum Reference Frame and restricted area features are not saved in 3D XML files, as they are useless for review process.
  • The 3D annotations of .model and .cgr documents are not taken into account.
  • Both the check boxes Under Geometric Feature nodes and Under View/Annotation Plane nodes, in Tools> Options> Mechanical Design> Functional Tolerancing & Annotation> Display must be cleared before saving the document.
 

Display

When you open a 3D XML file containing 3D annotations, they are not displayed.


When the 3D XML has been created from a CATProduct document, to display the 3D annotations both in the 3D window and in the specification tree:

  1. Activate the root product of your document.

  2. Switch to the Product Functional Tolerancing & Annotation workbench.

  3. Click List Annotation Set Switch On/Switch Off .

  4. Click Enable All.

  5. Click OK.

When the 3D XML has been created from a CATPart document, to display the 3D annotations both in the 3D window and in the specification tree:

  1. Create a new CATProduct document.

  2. Insert under the root product the 3D XML document (Existing Component command).

  3. Be sure that the root product is activated.

  4. Switch to the Product Functional Tolerancing & Annotation workbench.

  5. Click List Annotation Set Switch On/Switch Off .

  6. Click Enable All.

  7. Click OK.
3D annotations contained in a 3D XML files have the following specificities:
  • they are not editable,
  • they cannot be moved,
  • they cannot be copied nor deleted.
  • their properties are not editable with the exception of their Lines and Curves properties (Color, Lintype, Thickness) that can be edited within the session but those modifications will not be saved.
 

Query

To access to the query capabilities:

Click 3D-Annotation-Query Switch On/Switch Off in Functional Tolerancing & Annotation,
Click Select   in DMU Dimensioning & Tolerance Review.

For both workbenches:

  • If you select a geometrical element, all the 3D annotations that are applied to it are highlighted. This capability is limited to 3D annotations defined at part level (leaf components of the product).
  • If you select a 3D annotation or a constructed geometry or a restricted area, all the geometrical elements it is linked to are highlighted. This capability is limited to 3D annotations defined at part level (leaf components of the product). 
    If frame dimensions are attached to it, they are highlighted too.
    If the 3D annotation is a geometrical tolerance with datum reference frame, the corresponding datum annotations are highlighted too.
  • If you put the mouse pointer on top of a NOA annotation or a flagnote annotation, the hidden text and hyperlink paths that are attached to it are displayed in a tool tip.
  • If you put the mouse pointer on top of a dimension with a fitting tolerance or with a general tolerance, the corresponding numerical upper and lower tolerances are displayed in a tool tip.
  • If you select an Aligned/Offset Section Cut/View in specification tree or in 3D, the 3D Aligned/Offset clipping according to the profile of the part or product is displayed.
  • If you select a capture that has a component of an Aligned/Offset Section Cut/View feature as active view and its Clipping plane option selected (in the capture Properties dialog box) the corresponding 3D Aligned/Offset clipping is displayed.
  • If you select a Text or Flag Note or Note Object Attribute annotation, all the geometric elements of the below listed geometric features it is applied to are highlighted.
     
    The following geometric features are highlighted:
    • All geometrical elements.
    • PartBody and Body features.
    • The following Part Design features: Pad, Pocket, Shaft, Groove, Hole and Rib.
    • Geometrical Sets and Ordered Geometrical Sets.
    • Axis systems.
    • User Features.
    • Technological Result features of Part Design Hole feature and User Features.
  • If you select one of the element of the above listed geometric features, all the Text, Flag Note and Note Object Attribute annotations that are applied to the geometric feature are highlighted.
  • If you select the By feature option in the Filter dialog box for least one geometric element of the listed geometric features, all the annotations that are directly applied to this geometric element or that are applied to its geometric feature, are put in show mode while all the other annotations are put in no show mode.
  • If you select a capture, the resulting display respects the show/hide mode selected for part bodies and geometrical sets (as in the Manage the visibility of Part instances, bodies and geometrical sets option in capture Properties dialog box). For more information, refer to 3D Functional Tolerancing & Annotation User's Guide: Managing Annotations Display: Managing Hide/Show in Captures.
  • Tolerancing Schema
    • If you select the Nx text in 3D or specification tree, all the geometric features, dimensions, tolerances and annotations that are linked to the tolerancing schema are highlighted.
      For more information on tolerancing user features, see 3D Functional Tolerancing & Annotation User's Guide: User Tasks: Using the Tolerancing Advisor: Tolerancing User Features Automatically.
    • If an annotation linked to Nx text is selected, the Nx text is also highlighted.
    • If you select the By feature option in the Filter dialog box for a annotation which belongs to Nx text, the Nx text and all the dimensions, tolerances and annotations that are linked to it are put in show mode.

For DMU Dimensioning & Tolerance Review:

  • Related Surfaces displays all the geometrical elements at least a 3D annotation is applied to, in the color of your choice.
  • Go to Hyperlinks opens the documents that are attached to flag notes or NOA.
 

Filter

Click Filter to filter the 3D annotations according to all the criteria that are proposed (note that only the ones that are relevant for the 3D annotations that are loaded in the V5 session are proposed):

  • All
  • None
  • By type
  • By sub-type
  • By value
  • By feature:
    • Annotation sets
    • Views
    • Geometrical elements
  • By default annotation
  • By capture (you can also display a capture by using the Display contextual menu command on capture feature).

  • Functional Tolerancing & Annotations features in 3D XML can be reviewed within 3D XML Player and 3D Live (without requiring the Live FTA Review license).

  • It is possible to export the assembly annotation set captures from V5 to a 3D XML document. These assembly annotation sets can manage visibility of part instances. For more information managing the visibility of part instance, see 3D Functional Tolerancing & Annotation User’s Guide: Customizing: View/Annotation Plane. You can review this 3D XML document in 3DEXPERIENCE platform.

  • If there is any new part instances visibility management information that is saved in 3D xml, it will be ignored in V5 review.