The new Model States functionality introduced in Inventor 2022 software has many uses within your Inventor design files. It was introduced as a replacement for the pre-2022 Level of Detail assembly functionality, and also provides an alternative to the iPart and iAssembly functionality. The content below has been updated to reflect the changes in the Inventor 2023 software, and is designed to accompany the webcast I delivered on using Model States. Click here to view my Inventor Model States webcast.
Model states have multiple uses within part and assembly files. Uses can include creating manufacturing stages, simplifying the display of an assembly for design work, or creating configurations of components in a design to represent various products. Model states can also be valuable when working with a large assembly to improve retrieval times and performance, or they can be used as a starting reference for model simplification. The model states shown in Figure 1 are examples of model states for part (top) and assembly (bottom) files.
Creating Model States
The process to create model states in parts and assemblies is similar. The following steps describe the process:
How to Create a Model State
1. In the Model browser, right-click on the Model States node and select New. If prompted, click OK to the message regarding the edit member scope setting. This is an informational message only. Alternatively, you can right-click on the model state you want to copy and select Copy. The model states, as shown in Figure 2 for a part and assembly, were created using the New option to duplicate the active Primary model state and are immediately activated once created.
2. Verify that the edit scope setting is appropriate for the model state customization that you will be doing. This setting determines if the change will affect only the active model state or all model states. By default, the edit scope is set for the current model state only and the (blue pencil) icon appears adjacent to its name.
- By enabling the scope () to affect all model states (as shown for an assembly in Figure 3), you can ensure that the change is made to all model states. When enabled, the (blue pencil) icon appears adjacent to all model state names, indicating that they will all be edited.
- Scope editing functions the same in both parts and assemblies.
3. With the new model state active, modify the configurable attributes for the part and assembly as follows to customize the model state. Once modified, each configurable attribute is assigned a column in the file’s internal model state spreadsheet.
- Suppress/unsuppress part or assembly features in the model state.
- Suppress/unsuppress components in the model state. Note: The bill of materials will list suppressed assembly components as a QTY 0.
- Modify the iProperties, as required, for the active model state. In the Model browser, right-click the model state name or the model name and select iProperties. To help identify model state properties from the primary model iProperties, color is used. Black text identifies the primary model iProperties, while blue is used to identity properties specific to a model state.
- Materials can be assigned to model states at the part level. To incorporate a specific part in the top-level assembly model state, the required part-level model state can be enabled as required.
- Modify parameters, as required, for the active model state. This can be done in the Parameters dialog box () or by showing dimensions in the graphics window and modifying them.
- In the Model browser, modify constraint offset values, as required, for the active model state.
4. Rename the model state using a descriptive name by clicking it twice (not double-clicking) in the Model browser and entering the new name.
5. (Optional) Once you have created one model state, you can use standard spreadsheet functionality to create additional model states or add customizable attributes. To open the spreadsheet, right-click on the Model States node in the Model browser and select Edit via Spreadsheet. Edit as required, save, and close. The model states update to reflect any new model states or edits to existing model states.
6. Save the file to save the new model state.
You can make changes to the model states once created. To do this, ensure that the required model state is active, verify that the edit scope setting is as required for the change, and manipulate them as needed. Once the edits are done, ensure that the file is saved.
Model States in Subassemblies
Subassembly model states can be enabled within model states in the top-level assembly. In these situations, the model state must already exist in the subassembly. You cannot create, edit, or delete subassembly model states within the context of a
top-level assembly (in place edit). To do this, you must explicitly open the subassembly in its own window to create/edit. For example, the Screw_Sub subassembly shown in Figure 4 is active in the context of the assembly. The right-click model states menu does not allow you to create a new model state.
Model States vs. iParts/iAssemblies
The model state functionality was introduced in Inventor 2022. It is a replacement for the
pre-2022 level of detail assembly functionality, and additionally provides an alternative to the iPart and iAssembly functionality (still available in Inventor). With the introduction of model states, the model state functionality and the iPart/iAssembly functionality become mutually exclusive. The model state functionality is enabled by default in all new parts and assemblies. If you are using previously created files, consider the following:
- If the file does not contain pre-existing iParts or iAssemblies, the model state functionality is enabled. Any level of detail representations that existed (assemblies only) are converted to model states.
- If the assembly contains pre-existing iParts or iAssemblies, the model state functionality is not enabled. Any level of detail representations that existed (assemblies only) are converted to design view representations.
The process of converting an iPart or iAssembly table that exists in a pre-2022 assembly to model states is manual. You can either delete the table and recreate the configurations using model states or you can use spreadsheets, as follows:
1.Open the file, right-click on the Table node in the Model browser, and select Edit via Spreadsheet.
2. With the spreadsheet open, copy the data or save the file to a temporary location.
3. Delete the iPart/iAssembly table. A Model States node appears in the Model browser, indicating that it is active.
4. Create a new model state in the file.
5. Right-click on the Model States node and select Edit via Spreadsheet.
6. Copy the data from the iPart/iAssembly table into the model states table to provide a starting point for your model states table.
Consider the following:
- Unlike iParts and iAssemblies, model states are all saved and managed in the one part or assembly file.
- To return to iAssembly functionality, only a Primary model state can exist in the file. To switch, on the Manage tab, click
(Create iAssembly) and create an iAssembly member. Once complete, the Model States node is removed from the Model browser and is replaced with an iAssembly table.
Model States and Autodesk Vault
Model states offer capabilities similar to those found in iParts/iAssemblies; however, all configurations are stored in a single file instead of multiple files. Additional Vault integration functionality is available for model states if your Vault Professional implementation includes items. If your Vault implementation does not include items, any file that contains model states will display the primary model’s properties (e.g., iProperties, parameters, etc.). If you require separate files that can be managed and released, consider using iParts and iAssemblies. For more information, see “Working with Model States and Vault Files” in the Vault Help documentation.
Substitute Model States
A substitute model state enables you to swap out a complex component for a simpler one that represents it. The substitute still contains all of the BOM information that is normally associated with the assembly, as well as the physical information (such as center of gravity and mass). Using substitute parts reduces the amount of components loaded into memory, as well as the number of constraints and adaptive relationships that must be recalculated when changes are made. By simplifying the model, the intention of a substitute model state is to reduce the computing resources and thereby increase performance without sacrificing access to BOM information.
The model on the left in Figure 5 shows the Primary model state for an assembly. A substitute model state for the fan and its electronic components is shown on the right. In this example, the substitute part was simplified using a simple cylindrical-shaped part; however, substitutes can also generate a part file with surfaces or merged solid bodies to help make the substitute model state simpler to help improve performance.
Create a Substitute Model State
1. Open the subassembly that is to be simplified. This assembly is called the Owning Assembly.
2. (Optional) Create a reduced-part model state for the subassembly. In this model state, suppress any subassembly components
that can be removed to help further simplify the assembly. This is not a requirement.
3. In the Model browser, right-click on the Model States node and expand New Substitute. Select one of the options as shown in Figure 6.
- The Derive Assembly option simplifies the assembly using the Derived Component functionality. A new part file is created that is then substituted for the assembly in the model state. The derived part is created in the same way as one that uses the Derive tool. You define its name, template, and location, and then use the Derived Assembly dialog box to control which components are included in the new part file. The new substitute model state is created using the new derived part file.
- The Simplify command creates a simplified substitute part that represents the active assembly and uses that part in a substitute model state. The simplified substitute part is created in the same way as the one that uses the Simplify tool. The new simplified substitute part is automatically created, and a substitute model state is created.
- The Select Part File option substitutes a single part file for the assembly. Selecting Select Part File substitutes a selected file for the assembly in the substitute model state. The part file can be a previously simplified assembly, simplified model, or another part file. After you select this option, you are prompted to select a component. The substitute model state is created using the selected part file.
4. In the main assembly, create a new model state and activate the substitute model state in any subassemblies, as required. Please note that when the substitute model state is active, a number of commands on the Assemble tab will be disabled (gray).
Using Model States in Drawings and Presentations
Any model state can be selected for use while creating base drawing views. When modifying the parent view, you can also change the model state that is active by editing the view. When creating a base view, select the required model state name from the drop-down list, as shown in Figure 7. To change the model state that is used in a base view, right-click on the view, select Edit View, and select a new model state name. All views that reference it will also update. With the release of Inventor 2023, model states can be used for Overlay. Hint: If you want an isometric drawing view to have a different model state than a 2D base view, create the isometric view as a new base view and orient it as needed.
Assembly Parts Lists
Drawing parts list tables must be associated with a view when created. If the view has been set to represent a model state, the parts list will reflect this. If components are suppressed in the model state, their QTY value will report appropriately. If a component does not exist in a model state (i.e. is suppressed), it will still show the component as an item and will have QTY 0, unless the BOM Setting () option Hide Suppressed Component in BOM has been enabled in the Bill of Materials dialog box. If this option is enabled, all components with a QTY of 0 will be removed from the Parts List.
Figure 8 shows a drawing sheet with two different model states documented. The 2D views show the parts list with one Vise assembly. The isometric view’s parts list shows all 4 vise components are included.
A general table can be used to show all of the model state details for a drawing model’s configurations. To create this table, complete the following steps:
1. Click (General Table) on the Annotate tab to open the Table dialog box.
2. Select the drawing view that will be the source for the table. The view can be the primary or a model state configuration of the assembly.
3. In the Columns and Rows area, select (Column Chooser).
4. In the Table Column Chooser dialog box, select the columns that you would like to include in the table from the Available
Columns list and move them to the Selected Columns list using the Add option. The list will include all of the configurable items
that were modified in the model states (e.g., dimensions, parameters, components, etc.).
5. Click OK twice to create the table and add it to the drawing.
6. (Optional) To customize the column names, double-click on the table to edit it, right-click on the column name, and select Format Column. In the Format Column dialog box, you can disable the Name From Data Source option and enter a custom name for the column.
Figure 9 shows the columns that were added to the general table for a part and the resulting drawing table that was created. In the table, the column headers were customized to have descriptive names using the procedure described in Step 6 above.
Consider the following when working in a drawing with model states:
- If a design change is made to a model state that is used in a drawing view, it will update to reflect the change when it is opened next. Any associated parts lists or general tables will also update.
- The model state assigned to a view can be switched by editing the view and selecting an alternate in the Model State
- A view can be modified to replace its reference model (and its model state) using the (Replace Model Reference) option on the Manage tab. In the Replace Model Reference dialog box, select the file that is being replaced, select , select a new file, and click Options. In the File Open Options dialog box, select the required model state. Once the file is replaced, the view and associated parts lists will update.
- If a substitute component is used in the model state to represent an assembly, it is still identified as a single item to provide an accurate BOM and parts list.
Using Model States in Presentations
A model state can be selected for use while creating scenes in a presentation file using either of the following methods:
- With the model state active in the assembly, right-click on the assembly name in the Model browser and select Create Presentation, as shown in Figure 10. In the Presentation Template dialog box, select the required presentation template file and click OK. A presentation scene of the selected model state is immediately created.
- Using the New option to create a presentation file, you can select the template and when prompted to select the assembly, select the assembly name and click Options at the bottom of the Insert dialog box. In the File Open Options dialog box, select the required model state for use in the presentation scene, as shown in Figure 11.
- When creating new scenes in a presentation, use Options at the bottom of the Insert dialog box to access the File Open Options dialog box to select a different model state.
About the AuthorFollow on Linkedin More Content by Jennifer MacMillan