Working with the Assembly Requirements Model

This task shows you how to create an assembly annotation set.
This functionality allows you to store annotation features created in assembly when working with ENOVIA V5.

Purpose:

  • All the annotations created a product and contained in its Annotation Set cannot be stored in ENOVIA V5.
  • An Assembly Annotation Set can be created in a part document and allows you to store the assembly annotations and their associated geometries as reference.
  • Annotations between the assembly components must be created in part context (edition of the part containing the Assembly Annotation Set in the Functional Tolerancing & Annotation workbench.

Assembly Annotation Set
Open the GEAR-REDUCER.CATProduct.
 
You can create all types of annotations, which are possible in normal Annotation Set. Additionally you can create assembly level annotations under the part.
 

  1. Create a new part or edit the existing given part.

  2. Select the Functional Tolerancing & Annotation workbench (part context) if needed.

  3. Click Create Assembly Set .

  4. The Assembly Annotation Set Creation dialog box is displayed where you can give a name for the Annotation Set to be created. The default name given is Assembly Annotation Set.1. Click OK.
    • If there is no existing Annotation Set in the part, an Assembly Annotation Set is created:
      • Annotations between the assembly components will be created inside.
      • The selected geometries for the annotations will be imported inside the part as reference.
      • Annotation concerning the part will be created in this Assembly Annotation Set.
    • If an Annotation Set already exists in the part, it can be converted in an Assembly Annotation Set, but this operation cannot be undone.
      • Exiting annotations in the Annotation Set are kept.
      • Annotations between the assembly components will be created inside.
      • The selected geometries for the annotations will be imported inside the part as reference.
     
    This command is only available in the Functional Tolerancing & Annotation workbench (part context).
       

  5. An annotation set is created.


     

  6. Now create an annotation. For example create dimension between two surfaces. Click Dimensions  in the Annotations toolbar and select the surfaces as shown below.

    The dimension is created.


     
  7. While running an feature creation command, when working in an assembly annotation set, you can select geometry that is not inside the part you are editing but anywhere in the session assembly. Thus on selection of assembly geometry, the selected geometry is automatically imported inside the Assembly Requirements Model (ARM) part. Note that only the selected feature geometry is imported, not the complete body.
  8. If the Keep link with selected object option in Tools>Options>Part Infrastructure, General tab is selected, the geometry is imported with link (making this link visible in ENOVIA Product Editor and VPM Navigator as a contextual design link) and is displayed in an “External References” node in the feature tree.

    If the Keep link with selected object option is not active, the geometry is imported without link and is put inside the in work (white underlined) body or geometrical set in the feature tree. 

  9. If the Confirm when creating a with selected object option in Tools>Options>Part Infrastructure, General tab is selected, then everytime a link is created between two elements a message box prompts you confirm if the link should be created.


     
  10. If you modify the initial assembly geometry by editing the corresponding part or moving the part instance inside the assembly, the ARM part will be turned to not up to date. Run the update command to update the assembly.
  11. Now this assembly can be saved in ENOVIA for further use if required.