Data Exchange > Creo Legacy Migration > Creating Model-Drawing Pairs > To Map a Drawing to a Model and Create a Drawing-Model Pair
To Map a Drawing to a Model and Create a Drawing-Model Pair
1. Import one or more 3D models that belong to the CATIA Direct V4, CATIA V5, IGES, Parasolid, STEP, or NX formats. You can, alternatively, open CATIA, NX, and SolidWorks parts and assemblies as non-Creo models in Creo Parametric.
2. Import the drawing files of the part and assembly models, preferably as .igs files.
3. Create a mapping file with a list of comma-separated model and drawing names.
4. Specify the mapping file as the value of the lda_map_file configuration option.
5. Open one of the .igs files with Import Associative Dimensions selected in the Import IGES dialog box.
6. Click the Legacy Migration tab and click Map > Add Model or right-click the drawing and click Add Model to associate the model that you imported or opened as a non-Creo model with the drawing in session. Models with the same names as the drawings or drawing and model pairs specified in the mapping file are automatically mapped. Legacy Drawing Associator (LDA) automatically locates and opens the model file with the same name as the drawing in session. The Model Tree appears displaying the model entities.
If LDA fails to locate the model or if the model and its drawing have different names, the Open dialog box opens. Browse and select the model file of the drawing in session.
Click In Session in the Common Folders pane of the File Open dialog box to select the model from session.
7. If there are no views on the drawing or if you require additional views, click Views > Create 2D View to create views on the drawing.
8. Click Map > Create Model Views or right-click the drawing and click Create Model Views to automatically map the 2D views in the drawing, including the auxiliary views and the new views, to the corresponding 3D views on the model.
If LDA fails to map all the views, you can perform the following tasks to map the 2D views on the drawing to the 3D model views:
Click Views > Orient View or right-click the drawing and click Orient View to orient the 3D views of the model relative to the 2D views of the drawing. This task is optional.
Click Views > Match View or right-click and click Match View to place the 3D model views relative to the 2D views and associate the 2D views to the 3D model views.
9. Use commands on the Model Views tab to place or specify the following view types on the drawing:
General view
Projection view
Detailed view
Auxiliary view
Revolved view
Copy and Align view
10. Click Model Views > Drawing View and select a drawing view to see the view details in the INFORMATION WINDOW.
11. Click Map > Copy Annotations or right-click and click Copy Annotations to automatically create copies of the legacy annotations and map them to the associative annotations in the mapped views. The ordinate dimensions are mapped with their baseline references as associative ordinate dimensions.
12. Use commands on the Annotations tab to create the following types of dimensions, tolerances, notes, and symbols:
Standard dimensions
Ordinate dimensions
Reference dimensions
Geometric tolerances
Various types of notes
Surface finish symbols
13. Click Annotations > Symbol and click the adjacent arrow to access the following symbol insertion and definition commands:
Symbol From Palette to insert free-placement or on-entity symbols and their instances from the Symbol Instance Palette: draw_symbol_palette.
Custom Symbol to create custom instances of the associated symbols using the Custom Drawing Symbol dialog box.
Symbol Gallery to define new symbols or redefine, delete, and save existing symbol definitions using the SYM GALLERY menu.
14. Right-click the drawing and click Update Sheets to update the views on the drawing sheets for any model changes.
15. Click Utilities/Settings > Validate Association or right-click and click Validate Association to open the Validate LDA Associations dialog box and verify the mapping status of the 2D entities on the drawing. You can perform the following tasks in the Validate LDA Associations dialog box:
Select an entity listed in a column of the Validate LDA Associations dialog box to cross-highlight and zoom the entity on the drawing.
Select Dimensions and Notes on the Validate LDA Associations dialog box and click Show unmapped to check for legacy dimensions and notes that are not mapped.
Click the check-box adjacent to each entity in the Checked column after you verify its mapping status.
Click Move to solid view or right-click and click Move to Solid View to move the dimensions, notes, and the 2D entities that are not mapped to a view on the drawing.
16. Click Close on the Validate LDA Associations dialog box.
17. Select an unmapped legacy dimension or note, click Annotations > Match Annotation, and create a draft dimension or note to match and associate the legacy dimension or note with the draft dimension or note.
18. Click Utilities/Settings > Clean Up to remove the mapped entities from the drawing and place the entities on a layer that you can subsequently blank.