How to create and manage model views
Inventor representations are named configurations. They manage views, component visibility, component position and many other things. Because they are representations, you can restore them and their settings at any time.
View representations store view-related information. Use these to manage the display of your components. They aid the design process, prepare presentation type information and improve the performance of Inventor.
I delivered a class at Autodesk University on View representations in 2018. Using View representations (properly) is just as useful and important today as it was then.
With parts and assemblies, what do View representations capture? They store component and body visibility (as in visible or invisible), transparency and enabled status. They capture appearance (color and other style characteristics). They also manage sketch and work feature visibility and camera-related items like the camera view, viewing angle and zoom magnification.
There are no restrictions on View representations. You can create as many as you need to work effectively.
Unlike Model States, View representations do not alter the bill of materials.
Working with View Representations
You create and manage View representations with the Inventor Model browser. Double-click a representation to activate it and then click twice slowly to rename it. All other options are available via the right-click menu.
Right-click the View browser node and select New to create a new representation. Inventor inserts the new entry and waits for you to set its name. The new representation is automatically set as active.
When right-clicking on an existing representation, use:
- Copy to duplicate the representation and make it active
- Publish to include the view representation in 3D PDF and DWF exports (these are enabled when you see the checkmark)
- All Visible to make all components visible
- All Hidden to hide all components
- Content Center Visible to make all content center components visible
- Content Center Hidden to make all content center components invisible
- Remove Appearance Overrides to restore all component appearances to their default appearances
By default, View representations are live. The active representation automatically updates as you adjust the viewing information. Right-click on the representation within the browser and select Lock to prevent changes. Components added with a locked representation active are made invisible when you restore the representation.
Consider using View representations to turn off components or bodies to simplify the current task or to build display configurations showing only the required components. They can manage the visibility of welds in a weldment. Use them to save in-progress assembly views to preserve working ideas. They can also control sketch and work feature visibility to reduce the clutter on the screen.
View representations are also a great tool for storing viewing angles and zoom factors to return to at a future time—convenient for presentations or sales-type views. Use them to assign transparency to components you want to see through in the display or in drawing views.
Other Features
From the right-click menu, you will also find Copy to Model State. This creates a new Model State configuration, automatically suppressing (unloading) invisible components. Because Model States impact the bill of materials (BOM), the suppressed components will also be excluded from the BOM.
Pro Tip: Many of Inventor’s selection tools work better with component visibility than suppression. It can be easier to first capture visibility with a View representation. Then convert this to a Model State using Copy to Model State.
When the Camera View is set to AutoSave any adjustment to the view (pan, zoom, etc.) is automatically captured by the view representation. This is the default mode. By saving the current camera, Inventor takes a snapshot of the view. Regardless of view manipulation that occurs when the representation is restored later, it restores to the snapshot.
With each representation, you can select its own annotation scale. The annotation scale manages the size of 3D annotations in the model.
You can use View representations to build display configurations that have only the appropriate component visible. With parts and assemblies, you can employ further use of representations to manage the visibility of 3D annotations. When you use different representations, only the desired annotations are visible when needed.
Pro Tip: When a component is made visible, it loads into memory. However, making a component invisible does not unload it from memory. To unload unneeded components, you will need to close the document and reopen it with a specific View representation.
Edit View
Edit View provides a different way of changing View representations. As opposed to working within the browser, with Edit View, you manage component visibility in the graphics window.
This starts in the View All state, graphically showing all components within the model. Selecting a component includes it in the View representation, making it visible.
Change to View Excluded, graphically showing only the invisible components in the View representation. Selecting a component will then include it in the View representation, making it visible.
Use View Included to graphically display the visible components. Selecting a component will then exclude it from the representation, making it invisible.
Another application of View representations is with multi-user projects. Each user can have their own view focusing on specific areas of the assembly.
Using View Representations
When opening an assembly, you can specify the View representation Inventor will use as the model is opened and loaded into memory. By default, the last active View representation is used.
Inventor includes options to open the assembly with all components visible or nothing visible. If you have an assembly of 500 components but need to work on two, why not open the assembly with nothing visible and turn on only the two you need? This way only the two parts are loaded into memory.
Place subassembly using a selected View representation: It is advantageous to place a subassembly with a specific View representation. This can be a good approach when you want to show only what is needed.
Assembly View representations can manage the applied component representations as well. For example, here they are subassemblies.
Pro Tip: Lock the View representation and enable associativity to manage when new component instances in the assembly also appear in the drawing view.
Use View representations to create drawing views. Use the simplified View representations to show only needed components or to show components with the desired appearance, thus aiding in documenting the components.
Speed up drawing view creation by turning off components not visible in the camera, such as the internal components.
Pro Tip: To take advantage of performance benefits and memory savings to create the needed View representations in the assembly. Then close the assembly so that its graphics are not loaded into memory. Now create the drawing and when you create the drawing view, select the View representation displaying only components that you want to see. Remember, invisible components in the View representation are not loaded into memory. This will improve performance.
Parts List Filtering: Create unique views to filter the parts list in a drawing. For example, you can do this to document an assembly procedure.
Pro Tip: Create as many View representations that are needed but name them appropriately. It is frustrating to work on a design when there are no hints about what the View representation is used for.
Prepare the assembly for simplification by building views that include only those components required. Think of this as the simplification starting point.
Turn off the unnecessary components, leaving only those required for the motion analysis. You can further use these views when creating Overlay views to highlight just the components affected by the positional representation.
Use Inventor’s Selection Tools to Your Advantage
An underutilized tool set in Inventor is its selection tools. Using these features will streamline the selection process, making it easier to select components.
A good example is the All in Camera selection method. This selects only the components you can see. This is great for reducing the number of components in a drawing view. This works for assembly drawings because you typically do not include the hidden lines.
Design View Associativity
When inserting a component into an assembly, it can be associatively tied to its View representation. This means changes to the component (like turning parts on/off or changing appearances) automatically updates the instances in the assembly.
When making in-context changes to this component, you are now asking it to go against the associative View representation. Because Inventor is not sure what to do, it prompts you.
By selecting Remove Associativity, the component is no longer associated with the View representation. Changes to the component’s View representations will no longer apply to the instance in the assembly.
If you select Modify Design View Representation, Inventor will update the View representation. This is true not just for that instance but for the component, meaning that all instances will see the changes to the View representation.
Take, for example, this suspension assembly where one of the upper arms is placed with a View representation “HIGHLIGHTED IN RED” active and associative.
View representation changes to the upper arm will automatically be reflected in the suspension.
However, by making changes to component visibility or appearance in the upper arm from within the suspension, Inventor prompts you to either modify the associativity or remove it. If you decide to remove the associativity, the upper arm updates, but the changes are not sent back to the subassembly.
At any point, I can reset the View representation being used and make it associative, which will make the instance in the assembly appear as it does in the subassembly.
Associativity works the same within drawing views, when associative changes to the View representation are reflected in the drawing view. With drawings, only component visibility and appearance are managed by the View representation. Also, you cannot adjust component visibility from the drawing as it is being managed by the view.
