To Work with Drawings for Large Assemblies

How to avoid the performance degradation that can occur when working with drawings of large assemblies.

Drawing views of assemblies and parts are created in the same way. Because each drawing can have many sheets, you can develop a complete set of standardized drawings for the assembly and all of its components in a single drawing file.

Improving Drawing Performance

The following can improve drawing performance:

• Enabling background updates of drawing views. The Enable Background Updates option on the Drawing tab of Application Options quickly displays raster drawing views for large assemblies and calculates precise drawing views at the background as you work. You can review the drawing or create drawing annotations before calculating drawing views finishes.
• Using design view representations. Components rendered invisible in the design view do not load into memory. (The assembly file you want to make a drawing view of must be closed so that its graphics do not load into memory).
• Before starting the Base View command, clicking the Document Tab of the respective model to activate the appropriate document. This avoids calculating the base view preview for a different model. You can also close the last active model document, and select the source document manually.
• Selecting the Suppress option for several drawing views.

Improve Drawing Performance and Capacity

1. Click File Options.
2. In the Application Options dialog, click the Drawing tab.
3. Select Enable Background Updates in the Capacity/Performance area.

Note: If the Enable Background Updates application option is selected, raster views are displayed until calculation of precise views is complete.

Working with Raster Views

Raster views let you review a drawing or create drawing annotations while precise drawing views are calculated in the background. Raster views are marked by green corner glyphs in the graphic window, and by a special icon in the browser. A tooltip shows the progress of precise calculation.

Raster views turn precise automatically as soon as the calculation ends. The raster view icon is replaced with a regular drawing view icon in the browser. A separate process runs for each raster view until the view calculation is finished.

Precise drawing views use information from the model. If the model is not available or the drawing is in a deferred mode, the calculation is postponed, and the raster views do not turn precise.

While Inventor calculates precise views, you can annotate the raster views. For example, you can:

• Add dimensions, symbols or notes, tables, balloons, and parts lists.
• Create projected or other drawing views.

These features work differently for raster views:

• You cannot create automated centerlines, use the Auto Balloon command, or select model features as edges.
• Tangent model edges are always shown in raster views. You cannot edit their properties or visibility.
• Interference edges are never shown in raster views.
• Reference parts geometry can be incomplete in raster views.
• View and Feature options are not available for the Hole Table command.
• Thread features are not displayed in raster views. Existing thread notes attach to thread features after views turn precise.
• Printing raster views is not recommended because geometry on printed raster views can be different from the precise views.
• Export to AutoCAD DWG, DWF, DXF, or PDF cannot be finished for a drawing with raster views. If a view calculation is in progress, a progress bar is displayed. You can wait until the calculation finishes or cancel the Export.
• Drawings containing raster views can be saved and closed. On reopen, raster views are automatically recalculated as precise.

Use Model Representations to Improve Performance

Specify a simplified design view representation and model state before opening the model file.

1. Close the assembly file used for a drawing view to prevent its graphics from being loaded into memory.
2. On the ribbon, click Place Views tab Create panel Base.

   Click Open an Existing File , and locate and select the assembly file.

3. In the File Open dialog box, click Options and then select a model state and design view representation in the File Open Options dialog, and click OK.
4. Click Open to return to the Drawing View dialog box.
5. Specify the drawing view properties, and if appropriate, place projected views.
6. Click OK to close the Drawing view dialog box.