Creates a simplified single part representation of an assembly to improve capacity and performance in downstream assemblies or applications.
Simplify uses the derived component function in the background. It can use existing design view or model state representations for maximum efficiency. A simplified part includes only components that are visible in the graphics.
You can include one or multiple assemblies in a Simplify task, and schedule it to perform at a convenient time.
If a Simplify operation fails, the process skips the simplification for that assembly and starts the next one. Information about the failure is recorded in the log file.
- In the Inventor Task Scheduler window, click
Simplify Assemblies
.
The information in the task list switches to show any sequential tasks that you saved previously.
- In the Inventor Task Scheduler window, right-click, and select
Create Task
Simplify Assemblies.
- In the
Simplify 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.
- In the Task Properties box, enter a task name and a time-out threshold.
- Specify a schedule, or select the Immediately option.
- Select an assembly file row, and then click Options.
- In the
Simplify Options dialog, specify the required values.
Components tab:
- In Representation, select [Primary] or Last Active for Model State, Design View, and Position View.
- Optionally in Remove Parts, select Remove parts by size and specify the Max. Bounding Box Diagonal size.
Features tab:- In
Remove Features, specify the feature types (Holes, Pockets, Fillets, or Chamfers) you want removed from the simplified part. For each of the feature types you can select:
None of the feature types will be removed.
All of the feature types will be removed.
Remove by range all of the feature types. Those within the range you provide are removed.
Create tab:- In the
Style area, select one of the following options:
- Select
Single solid body merging out seams between planar faces to create a solid with no visible edges between planar faces.
- Select
Solid body keep seams between planar faces to create a single solid with visible edges between planar faces.
- Select
Maintain each solid as a solid body to create a multi-body part that contains a unique body for each part in the assembly.
- Select
Single composite feature
to create a surface composite body.
- Select
- In
Other Settings, specify any of the following:
- Break link to disable updates permanently and remove associativity between the parent assembly and the simplified part.
- Rename components to replace part names or numbers with generic values such as Part1 or Srf1.
- UseLink face color from source component to link color from the source component into the target part. If deselected, the appearance is set to default appearance of the target part.
- Use Link sketch format from source component to control if the sketch blocks in the derived part update if the lines in the source part are changed.
- Create independent bodies on failed Boolean to create a multi-body part when a Boolean operation fails on one of the single solid body style options.
Note: It is possible to produce gaps when small faces are removed. If gaps are present, the result is a non-manifold body.
- Remove internal parts is checked by default. Inventor looks at the model from 14 standard directions (six orthographic and eight isometric) to determine a parts visibility state. Parts deemed not visible are removed.
- Fill all internal voids to fill all internal void shells in the shrinkwrap solid body part.
- Create Substitute Model State using Simplify to create a model state representation using the simplified part in the parent assembly.
- Repeat the steps to set options for each assembly file listed.