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Project files organize Inventor data. Project files determine the location of the working data, templates, styles, and libraries.

Workspace should never be on a network location. It is intended to be local on the users’ machine. All work should be performed on files held locally and copied back to the network when finished. Failing to do this can have performance implications when saving all data across the network. Make the workspace local to each user’s machine.

Never define Workgroup or Library locations that point to subfolders of the Workspace or another Workgroup or Library.

For Example

• Workspace - C:\Damper

• Workgroup – C:\Damper\Section1

If the Workgroup or Library location is a subfolder of another defined location, Inventor will highlight the offending path in red. This will not prevent you from saving the project file. It is a warning that this does not produce the most efficient file structure.

The fewer Workgroup Search Paths defined the better. This makes searching for files much easier. Make your assembly structure flat. For example if you have an assembly file in a folder, place all idws of that iam in the same folder, in a subfolder place all the components in the iam. Inventor will use the “Subfolder Path” to locate the components it needs. If Inventor cannot find components immediately, it will continue searching which has a negative effect on performance.

For more information: Learn about projects

Resolve all constraint errors

Ensure that all errors related to constraints are resolved. Do this by opening ALL subassemblies first, resolving the problem in the subassemblies and then open the main assembly and address any errors. In a large assembly, attempting to resolve constraint errors in lower level subassemblies can be very time-consuming.

Work Geometry

Turn off the visibility of unnecessary work planes, axes, and points. The visibility of too many work features in an assembly can affect the performance. To quickly turn off all work geometry use View > Object Visibility.

Complex Features

Users should standardize on an amount of detail required to finish the design. Users may have very small components that have exceptionally high amounts of detail in the top level assembly. Standardizing on a simpler amount of detail will increase performance and capacity. Parts which require higher levels of detail can be created when needed. Our suggestion is that this only be done when the part meets some predetermined requirements. This helps engineers model only what is required to complete the design.

Coils or spring shaped parts can be resource intensive. Either replace these with simpler shapes or turn the visibility off. This is particularly applicable in drawings.

Similarly, it may not be necessary to display in full detail purchased parts. That is, simplify standard components externally sourced and inserted into an assembly, e.g. motors, actuators. Typically, the internal workings or details of purchased components are not necessary to complete your design.

Error Handling

Warnings- Inventor displays warnings when there is a problem.

Users should make all reasonable effort to remove warnings from an assembly before integrating it into production designs by using the Design and Sketch Doctors. Missing references & constraint failures are key warnings and will affect Inventor performance. While users can work with missing parts and failed constraints, it is not good practice to do so for extended periods of time. Inventor will find that something is sick, perform an audit and update it every time you switch back to that file. If all errors are removed, assemblies will behave more predictably and performance should increase.

Turn Off All Adaptivity

Leaving adaptivity switched on can reduce the responsiveness of Inventor. The adaptive components are frequently checked for re-computation. Therefore adaptivity should be turned off after a design is complete and turned back on when design changes are necessary.

Standard Parts

For standard parts that do not change, consider placing them in a project library directory. Inventor searches these parts in a different way than normal parts. Don’t change the name of the library directory once created. If the name is changed, each part in the library would need to be resolved.  

For more Assembly tips see: Increase performance and capacity

Fully constrain components or ground components that are not designed to move in your assembly. Assembly constraints require Inventor to perform a calculation. When there are a large number of components in an assembly and each component has multiple assembly constraints, these calculation times can become significant.

Avoid redundant constraints. Use the Application Option "Enable constraint redundancy analysis" to find redundant constraints then turn the option off.

Use a common constraint reference if possible.

Use Common Origin skeletal modeling for static assemblies. The productivity tools Place at Component Origin and Ground and Root are useful for Common Origin skeletal modeling.

Use the Design Doctor to find any constraint errors and fix the errors.

Turn off Adaptivity when not using it to design. Use Adaptivity for parts and Flexible for exercising degree of freedom of subassemblies.

For more information: Constraints

Level of Detail representations allow you to manage which components are loaded into memory and therefore manage the Inventor’s memory consumption. Level of Detail representations suppress components (parts or subassemblies) in an Inventor assembly. The suppressed components are not loaded into memory.

Use LOD representations when opening assembly files so that only the necessary components are loaded into memory.

For more information: Level of Detail representations

Assembly substitutes are a type of Level of Detail (LOD) representation. A substitute uses a single part file to represent an entire assembly.

There are three methods for creating substitute LODs:

• Derive Assembly uses the Derive command to create a part file to represent the assembly.
• Shrinkwrap uses the Shrinkwrap command to create a part file to represent the assembly.
• Select Part File allows you to browse and select a part file to represent the assembly.

For more information: Assembly Substitute Parts

Use View representations and LOD representations to control the amount of detail in drawing views. Even if some of the bodies are occluded in the final drawing view, the data is still loaded into memory to compute them unless representations are used.

Enable the background updates option in the Drawing tab of the Application Options. This option displays a representation of the view before it is completely calculated. You can continue working in the drawing while the view is calculated and even dimension the view.

Avoid or reduce the use of property overrides at the edge level. Use feature, body or component level overrides instead whenever possible.

Turn on Defer Update mode to reduce unnecessary updates to the drawing. This setting is on the Drawing tab of the Document Settings dialog box. View creation commands and some annotation commands are not available when Defer Update is active.

Set Use Bitmap to Always in the Drawing tab of the Document Settings dialog box and use the lowest resolution that provides the desired result. With this setting active, Inventor uses a cached bitmap image for shaded views instead of rendering the actual shading.

For more information: Develop drawings for large assemblies

The Engineers Notebook is a useful tool for communicating design intent. Be aware that creating a note containing an image embeds a bitmap into the ipt or iam file and increases the file size. The larger the file size, the more hardware resources are used. Therefore you should restrict the use of notes with images to minimize file size.

The Engineers Notebook is also in its own segment in memory which only loads if notes are present. Not having notes means that that segment doesn’t get loaded and reduces the amount of resources required.

For more information: Engineers Notebook

If you need to share parameters between parts, do not link them by an Excel Spreadsheet. When a change is made to the Excel file, Inventor cannot determine which files are affected, so all parts must be updated. This can slow down the performance of large assemblies. Instead, use the derive command to link the parameters into the parts. In this manner, Inventor can determine which parts are affected by a change and only update those files.

For more information: Parameters in models