You can choose model representations defined in the assembly model to show in a drawing view, such as an exploded model display configuration or a PMI model view. Use the following process to create an isometric drawing view of an exploded assembly with a ballooned parts list. You can do this from the assembly model or from a draft document.

1. Start the Drawing View Wizard

   In the assembly document, do the following:

   1. Save the assembly document.

   2. From the Application menu, select the New→Create Drawing command.

   3. In the Create Drawing dialog box, select the Run Drawing View Creation Wizard check box and click OK.

2. Choose an assembly model representation

   In the Drawing View Creation Wizard (Drawing View Options), select one of the following from the .cfg, PMI model view, or zone list:

   • To create an exploded isometric model view, select an exploded model display configuration , and then click Finish.

     To learn how to create an exploded model configuration, see Explode an assembly automatically.

   • To communicate design, manufacturing, and functional information that has been added to a saved view of the model, select a PMI model view name , to Create a PMI drawing view.

     To learn how to create a PMI model view, see Create a PMI model view.

   • To create a user-defined view of the equipment and components in a rectangular area of a large assembly model, select a zone name , and then click Next.

   • If there is no predefined model representation to select, or to create any combination of user-defined assembly views, select No Selection, and then click Next.

3. Place a user-defined view on the sheet

   If the Drawing View Creation Wizard (Drawing View Orientation) page is displayed:

   1. Select a named view, such as isometric, as the principal view.

   2. Click Next to choose additional views, or click Finish.

   3. Click the drawing sheet to place the view(s).

   Tip:

   Predefined PMI model views and display configurations are placed on the drawing automatically.

4. After placing the view, you can do any of the following:

   • Adjust the assembly display

     Use the Display page (Drawing View Properties dialog box) to control the display of the individual parts and subassemblies in the assembly.

     To learn more, see Creating drawings of assemblies.

   • Retrieve model dimensions and annotations

     • If the drawing views are orthographic, you can use the Retrieve Dimensions command to extract dimensions and annotations from the model onto the drawing.

     • If the drawing views are pictorial (isometric, dimetric, or trimetric), you can use the Smart Dimension command to Place a 3D dimension on a pictorial drawing view.

5. Add a ballooned parts list

   Use the Home tab→Tables group→Parts List command to Create a parts list.

   Tip:

   • To place a parts list that shows the assembly model item numbering schema in the table and in the balloons, select the Use assembly generated item numbers check box on the Options page (Parts List Properties dialog box. If this option is unavailable, you need to set the Create item numbers check box on the Item Numbers page (Solid Edge Options dialog box).

   • You can rearrange balloons that have been generated automatically with a parts list, so that all of the balloons are visible. To learn how, see Stack balloons.

   • If parts are missing in a parts list or a drawing view for an assembly, verify that the missing parts are not turned off in the assembly document Occurrence Properties dialog box. To learn how, see Display assembly occurrences in a drawing view or parts list.

   • You can create a drawing view of an alternate assembly