Tips for Advanced Assembly Control

At Autodesk University 2014 I co-presented the class “Advanced Assembly Control with Representations” within Autodesk Inventor®. This class was an overall success as there is so much to learn and share about representations.

Inventor representations can have a big impact on your day-to-day experience with Inventor. Representations are used to capture “snapshots” of your assemblies in various states. Representations aid in managing the visibility, suppression, position, and several other characteristics of components within assemblies. Representations enable you to save specific views of your assembly to prepare for presentations and to create drawings. Proper use of representations also significantly improves computer performance when dealing with large, complex assemblies.

There are three types of representations in Inventor: View, Positional, and Level of Detail (LOD).

Design View Representations

What are View Representations?

View representations capture view-related information. This information is stored in a named configuration that can be restored later.

Assembly view representations capture the following:

Component Visibility (as in on or off)
Colour (and other style characteristics) of individual components within the assembly
Sketch & Work Feature Visibility
Zoom magnification and viewing angle

TIP: Use view reps to simplify the geometry used in Overlay views to show only the components effected by the positional representation.

View representations are used to:

  • turn off component visibility (as needed) to simplify the current task.
  • capture viewing angle and zoom factor to return to at a future time. Convenient for presentations.
  • assign a unique colour to a component instance (say, opaque—see through one instance).
  • control sketch and work feature visibility to reduce the clutter on the screen.
  • simplify positional representations by turning off all unnecessary components.
  • help manage multi-user projects in that each user can have his or her own design view focusing on specific areas of the assembly.

TIP: Creating drawing views within Inventor can be quite time consuming, especially for larger assemblies. Improve performance by reducing the number of components within the view that Inventor has to work with.

Working with View Representations

Use the Inventor browser to create and manage view representations. All options are available via the right-click menu.

  • To create a new view rep, right-click the Master View Rep and select New.
  • Double-click to activate the view rep, click twice slowly to rename.
  • View representations are “live” in that they update automatically as the viewing information of the assembly is adjusted.

TIP: Lock view reps to prevent any changes. To lock a view representation, right-click on it in the browser and select Lock.

When opening an assembly you can specify the view rep that will be active as the assembly is opened. By default, the last active view representation is the one used.

When creating drawing views you set the view representation to manage the component visibility in the view.

If the view rep is set to associative:

  • the drawing view will update as the assembly view rep is adjusted.
  • you cannot adjust component visibility within the drawing view from within the drawing’s browser.

IMPORTANT: Create as many view representations as required for your assembly, but rename them appropriately. The default names Inventor gives new view reps (View1, View2, etc.) are NOT acceptable!

Design View Associativity

When you place a component into an assembly, the component remains associated to its view representations. This means that changes to the component (as in changing workfeature visibility or turning parts on/off) automatically updates the instances of the component in the assembtly.

When you make a change to this component in context of the assembly, you are really asking it to go against the view rep with which it is associated.  Because Inventor is not sure what to do, it prompts you as shown in the figure above.

If you select Remove Associativity, the component will no longer be associated to its own view representations. You will see your changes in the assembly, but any changes to the component’s view reps do not apply to the instance in the assembly.

If you select Modify Design View Representation then you are updating the view rep not just for that instance, but also in the component itself. This means that anywhere that component is used will see the changes to the view rep.

Take, for example, where the brace assembly is placed into the assembly so that the view rep in assembly is active and associative.

Any view rep changes to the brace are automatically reflected in tractor assembly.

However, if I make changes to the visibility of components in the brace from within the tractor, I am prompted by Inventor to either modify the associativity or remove it.

In this case, I decide to remove the associativity. This means the canopy brace is updated, but the changes are not sent back to sub-assembly.

At any point, I can reset the view rep used and make it associative, making the instance in the assembly appear as in the sub-assembly. Any changes I made to sub-component visibility within the assembly will be lost as the components view rep will set the visibility details.

Positional Representations

Positional representations capture "snapshots" of assemblies. Use these snapshots to review motion and evaluate the position of assembly components in both the modeling and drawing environments.

Positional representations allow us to display different positions of the assembly components. The Master Positional Representation (automatically created) represents the default state of the assembly, where your modeling operations take place. You cannot edit the master positional representation,

Creating a new positional representation allows us to make changes to the component positions and constraint settings without affecting the original component positions in the master. For example, a hydraulic cylinder can have a retracted and extended position

The following steps are used to create a positional representation.

Create a positional representation.
Modify (override) values for the positional representation.
Save the changes in the assembly.

Creating Positional Representations

To create a new positional representation, expand the Representations folder in the Model browser. Right click and select New, expand the position branch to view the master and the new positional representation.

Modify (Override) Values for the Positional Representation

Make the desired positional representation active before assigning overrides. Double-click the positional rep within the browser to make it active. Locate the constraint that needs to be modified in the Model browser, right-click and select Modify (Override). When the Override Object dialog box appears, adjust the values as shown in the figure below.

What Can (or Can’t) I Do With Positional Representations?

You cannot perform the following operations when a positional representation is active.

  • Add or delete components
  • Restructure the assembly
  • Adjust a pattern
  • Create (or delete) work features
  • Create, modify, or delete assembly features
  • Toggle adaptivity

IMPORTANT: Be careful with your level of details when working with positional reps. You do not want to suppress components constrained by the constraints you are overriding as this will cause you nothing but grief and headaches.

Save the Changes in the Assembly

When a positional representation is active, you are not able to save any changes to an assembly.

To save the changes in the assembly, activate the Master in the top-level assembly.

Level of Detail (LOD) Representations

To deal with large assemblies, Inventor uses an Adaptive Data Engine built on a segmented database. This database organizes the data for quick retrieval and segments the data so only the required data is read from the disk. When opening an assembly, Inventor only loads what is absolutely necessary.

As Inventor assemblies get larger (as in the number of components) and the components within that assembly get more complex, Inventor requires more and more memory (both video and RAM). Levels of detail representations provide tools to help manage the RAM usage of Inventor by reducing the complexity of the components in the assembly and reducing the number of components in the assembly.

The easiest way to remember the difference between view representations and LODs is that view reps capture the “look” of a component whereas level of details are for assembly performance, capturing whether the component should be loaded into memory.

Working with the Standard Level of Details

Level of detail representations are created and managed within the Inventor browser. All options are available via the right-click menu.

TIP: Parts and subassemblies cannot be suppressed without a level of detail. If you do not create a LOD prior to suppressing components, a LOD will be created for you. These autocreated LODs will be prefaced with a ~

Each assembly has four built-in LODs: Master, All Components Suppressed, All Parts Suppressed, and All Content Center Suppressed. These are defined below.

  1. Master is the default LOD. This LOD will always show each assembly and part “as is” with no components suppressed.
  2. All Content Center Suppressed will suppress any component originating from the Content Center.
  3. All Parts Suppressed suppresses all parts, but leaves the sub-assemblies unsuppressed.
  4. All Components Suppressed suppresses everything—all parts, all sub-assemblies.

TIP: Level of details can be nested in that an assembly LOD can call a sub-assembly LOD.

The advantage of using All Components Suppressed is that any assembly, regardless of the number of parts, can be opened almost instantly. Once open, additional LODs can be created to unsuppress the components you wish to work on/with.

TIP: The Bill of Materials (BOM) will always show the master LOD. You may notice when accessing the BOM that Inventor loads in all of the components. This means that it may take longer than normal to access the BOM as it is loading components into memory.

Setting the LOD on Open

The active level of detail can be set as you are opening the assembly. This is a great way to decrease the time it takes to open an assembly. For example, use the All Parts Suppressed LOD to open the assembly almost instantly. You can then unsuppress the components requiring changes.

LOD and Mass

When working with LODs you may be prompted on how you want to deal with the mass properties. You have the option to calculate the mass properties for the active LOD, meaning any suppressed component will be ignored. Alternatively, you can calculate the mass properties for the master level of detail even though you have a different LOD active.

Linking LODs

Within the Productivity Tools area of an Inventor assembly is the Link Level of Details functionality. It "provides the means to select a named Level of Detail representation from the active assembly, and activates a Level of Detail representation with the same name within subassemblies containing a Level of Detail representation with that name."

TIP: The names of the LOD must be spelled exactly the same and must be in the same case (uppercase or lowercase lettering).

Creating Level of Details

LODs have three main types:

  1. Component suppression
  2. Substitute – assembly simplification
  3. Component substitution

Component Suppression

The simplest option, this type of LOD captures component suppression. With the LOD active, suppress components by selecting on the screen or in the browser, right-clicking, and selecting suppress.

TIP: Suppressed components cannot be selected on the screen and are represented in the browser greyed and with a line through them as shown in the figure above.


By creating a new Substitute LOD you are creating a new part that will be used in place of the assembly component. On top of reducing the number of components, the creation of this substitute provides options to simplify the part.

When generating a derived assembly you control which parts are included, how they are included, and whether a solid or a surface model is generated.

  1. Derive Style: Solid – No Edges/Merge Seams, Solid – With Edges/Maintaining Seams, Multi-body Solid, or a Surface model
  2. Derived Type: To include or exclude the component or to perform a Boolean operation (use the component to subtract/union/intersect). Select the icon to set the operation for the component. The default is the yellow “+”, which means the component is included and added to the substitute
  3. Use the Representation tab to select pre-existing representations (view, positional, or LOD) on which to base the new substitute.

The shrink-wrap option can be thought of as covering the outside of your assembly in shrink wrap. This shrink-wrapped representation is used as a substitute within the assembly as a level of detail.

  1. Output – either solid or surface).
  2. Simplification – Components can be removed based on percentage visible.
  3. Hole Patching – used to patch any cutout in the model (it doesn’t have to be circular). This is useful to simplify the part, but is optional.

Part Substitution (Select Part File)

The last option is to model a simplified version of the assembly as a stand-alone part file. This file is then selected when creating the level of detail representation.


Are large assemblies slowing you down? Do you need to quickly switch between different presentations of your assemblies? Are multiple people working on the data, each with a different area of concern? Do you need to test your design in various positions? The answer to all the above is to start using representations.

Hopefully this quick guide to representations gets you up and running with representations within Inventor quickly, but also efficiently. Representations are a key aspect of using Inventor assemblies to their fullest potential.

Mike Thomas graduated with the honor of Most Distinguished Graduate in CAD/CAM engineering technology from the Saskatchewan Institute of Applied Science and Technology (SIAST). He is a specialist in the manufacturing industry with a strong knowledge of the Autodesk, Inc., mechanical products, and he has a solid understanding of document management, hardware, networking, and other Autodesk technologies. He is now the technical services manager for Prairie Machine & Parts Mfg. (PM&P), and he is responsible for overseeing the engineering department’s technical operations and strategic technical growth. His primary duties include providing ongoing support of critical computer systems and programs, facilitating the interactions between the engineering department and other departments, providing the engineering department with effective systems and technology, and working with PM&P's vice president and engineering managers on the development and implementation of a cohesive strategic plan for the technical growth of the department. Mike is an active contributor to Design & Motion (

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