To Shrinkwrap Assemblies with Task Scheduler

Creates a simplified single part representation of an assembly to improve capacity and performance in downstream assemblies or applications.

Shrinkwrap uses the derived component function in the background. It can use existing design view or Level of Detail representations for maximum efficiency. A shrinkwrap part includes only components that are visible in the graphics.

You can include one or multiple assemblies in a shrinkwrap task, and schedule it to perform at a convenient time. Then you can open your assemblies later using the shrinkwrap substitute levels of detail.

If a shrinkwrap operation fails, the process skips the shrinkwrap for that assembly and starts the next shrinkwrap. Information about the failure is recorded in the log file.

1. In the Inventor Task Scheduler window, click Shrinkwrap Assemblies .

   The information in the task list switches to show any sequential tasks that you saved previously.

2. In the Inventor Task Scheduler window, right-click, and select Create Task Shrinkwrap Assemblies.
3. In the Shrinkwrap Assemblies dialog, select any of these options:
   • Add Folder. Specifies a folder to include in the task. Your selection includes the folder’s Inventor files and their dependencies. To include subfolders, click in the Recursive column.
   • To specify individual files, click Add Files.

     You cannot change the output file name in this dialog.

4. In the Task Properties box, enter a task name and a time-out threshold.
5. Specify a schedule, or select the Immediately option.
6. Select an assembly file row, and then click Options.
7. In the Shrinkwrap Options dialog, select the appropriate settings:
   • Single Solid Body Merging Out Seams Between Planar Faces. When you merge seams between faces, the face assumes a single color.
   • Maintain Each Solid as a Solid Body. Creates separate solid bodies in the Shrinkwrap part that correspond to every individual part in the source assembly. For example, an assembly with five parts creates a part with five solid bodies.
   • Single Composite Feature. Retains colors and seams of the original components. Caches and retains the mass properties of the original assembly. Selected by default. Creates the smallest file on disk.
   • Patch All Holes. Removes all holes that do not cross surface boundaries, regardless of whether the holes are round.
   • Include Visible Work Geometry. Removes geometry that is not visible.
   • Create Independent Bodies on Failed Boolean. Creates a multi-body part when a Boolean operation fails on one of the single solid body style options.
8. Repeat the steps to set options for each assembly file listed.