With Autodesk Inventor, you can use Model States manage components. You can use Model States to show your designs at various sizes, the steps of production and the levels of simplification. You can manage parameters, suppression, iProperties and bill of materials (BOM) details for each model.
Model States serve three main purposes:
- Simplification, performance and IP protection
- Documentation
- Configuration
This is the second installment of a Model States series. In part 1, we looked at working with Model States and using them to manage configurations of parts and assemblies. Now we dive into using Model States for simplification, performance and IP protection. And explore the impact of Model States on your data in Autodesk Vault.
Model States for Simplification and Performance
Inventor segments its data. It loads only what it needs when opening an assembly. As you work on the assembly, Inventor continues to load data. As your assemblies get bigger (in terms of the number of components) and the components get more complex, Inventor naturally needs more and more resources.
Use Model States to improve capacity and performance. Why? To reduce component complexity and minimize the number of components.
States provide options for managing the memory usage of Inventor. By suppressing unneeded components, it removes them from memory. By replacing components with single-part representations, it reduces memory consumption and simplifies the modeling environment.
There are two simplification methods with Model States: Component suppression and substitutes.
Component Suppression
Component suppression is the simplest option. As you suppress components, the memory consumption goes down. The Capacity Meter highlights this behavior and displays it in the far-right corner of the interface. Use it to review the current memory consumption.
To improve performance with larger assemblies, use Model States to capture component suppression. By suppressing components, you reduce the number of components. What’s even better? Adding Model States to lower-level assemblies, which suppresses the unneeded or smaller detailed parts there as well. Working your way up to the top creates the best-performing model.
Pro Tip: Use consistent state naming (and be descriptive). Then use Link Model States to associate all states of the same name.
Substitutes
The detail needed to design or document a component is different when that component is used in another assembly. Consider the level of detail that is needed. Do you need to see the internal components? Do you need the hardware? How about all those holes and other features? Tailoring the level of detail ensures performance while allowing designs that are effectively designed and documented.
What about when you are sharing the model with someone else? What do they actually need to see? What shouldn’t they have access to?
Substitutes are new parts used in place of an assembly component. You replace one version (typically a more complex one) with another version (typically a simpler one). It keeps the rest of the assembly intact, including relationships and the BOM.
Substitutes can reduce memory load and recalculations, thus offering another method of improving performance. They also offer a way to protect your intellectual property (IP). By creating a simplified version, you can share only the relevant details without exposing the intricate details.
Inventor offers three substitute options: Derive Assembly, Simplify and Select Part File.
With Select Part File, you select an existing part to use in place of the assembly. The selected part can be a previously simplified assembly or just another part built as a simpler version.
Pro Tip: Save yourself extra work by modeling the substitute part using the same XYZ location and orientation as in the assembly. This avoids needing to reposition or constrain the part when it is placed into the assembly.
Derive Assembly and Simplify end with comparable results—a new single-derived part of the assembly.
In Inventor, a Derived Assembly is a part based on an existing assembly. It inherits the geometry of the original, but you can add features to it. Derived parts are useful for creating variations or modifications of existing components without altering the original file.
You start by specifying the new part’s name, the template and the file location. Inventor launches a temporary window and presents the Derived Assembly dialog. This dialog is the standard Derive dialog and is the same as when you are launching the command directly.
I like to work backward, starting with the Options and working left to the Bodies.
The Options tab includes choices to further define the simplification of the substitute.
Remove components by size, which uses the component volume rather than the overall assembly. And you can remove geometry by visibility, which hides components based on the percentage that are visible (all viewing angles). For example, using zero percent means that only components completely hidden are removed from the substitute.
Use the patching options to patch and remove holes within a set range. A hole is not just circular; it is any profile completely contained within a model face.
Enable color override from the source component to use the color overrides from the components, as opposed to the default appearance of the new substitute part.
More options:
- Reduce Memory Mode reduces the data stored in the part and is recommended to leave enabled.
- Use Create independent bodies on failed Boolean when you encounter issues creating the derived component. This shows the components that are causing issues.
- Remove All Internal Voids fills all internal void shells.
Use the Representation tab to select existing model states and representations (View, Positional). This sets component status (inclusion or exclusion).
Use the Associative option to keep the substitute linked to the selected representations. However, this can limit the options of excluding or including components as it is tied to the selected representation instead.
To create a derived part, you select the features, bodies, surfaces, sketches, work features and parameters to include or exclude from the resulting component. You do this on the Other and Bodies tabs.
Use the Other tab to select the sketches, work geometry and parameters for inclusion.
Use the Bodies tab to define the type of model created, the components included and how you want to include the components.
With the Derive style:
- Single Solid No Seams creates a single solid body with no seams (edges) between planar faces.
- Single Solid with Seams creates a single solid body that maintains the appearance of seams (edges).
- Multi-body Solid creates a multiple solid body part with a body for each component in the assembly.
- Single Composite creates a single (hollow) surface body. This option creates the smallest file.
Use the status to include or exclude components or to perform Boolean operations (as in using the component to subtract/union/intersect). The Derive Style sets which statuses are available. Use the following:
- Yellow plus (+) for inclusion, adding the component to the substitute.
- Gray dash (\) to exclude the component, removing it from the substitute.
- Red dash (-) to use the body to subtract, removing material where it intersects with other components.
- Green square to create a bounding box representation of the component, reducing memory consumption.
- Intersect to keep only the intersecting volume between the component and other components.
This results in a Model State, which is accessible in the browser as with all states. It does create a part, meaning you can open it and edit the Derive settings. You can also add features to further simplify the model.
Simplified Assemblies
Use Simplify to remove components and features from assemblies to protect your IP and improve performance.
If you have not used Simplify before, it helps to know that it uses the property palette interface. Unlike the Derive dialog, with Simplify, all features and options are in one place. You will want to work from the top down.
You can start with one of the four built-in presets to quick start the process. You can also create your own presets.
Use the Input section to set the Model State, View Representation and Positional Representation—if you want something different than what is active.
The Replace with Envelopes choices replace the components with simpler shapes. You set the level and shape for the encasing envelopes. Note, that feature selection tools become unavailable when you include envelopes:
- All in One envelopes the top-level assembly. This is the least amount of detail but is appropriate for establishing the keep-out areas.
- Top Level envelopes each first-level component.
- Each Part creates envelopes for each part in the assembly.
With Exclude Components, you can quickly include or exclude components from the substitute.
The first is by bounding box size. You set the maximum bounding box diagonal value and Inventor removes the components fitting within this box.
Or you can remove (exclude) parts by selecting them. You can toggle between selecting parts and components.
You can switch between viewing the excluded and the included components. This also toggles the result. When viewing the included components, you select the components you want to exclude. When viewing the excluded components, you select the components to include.
Pro Tip: Enable All Occurrences to select one instance and allow Inventor to select all occurrences of that component in the assembly.
The Remove Features options set the type and range of features to be removed. This includes excluding holes, pockets, fillets and chamfers.
None is the default. This means that no feature is removed. Select All to remove all features of that type of any size. When using All, you can use Preserve to select instances that you want to keep. With Pick Range, you define a size that removes all features that are the same size or smaller. Select Highlight to apply a color to the features that are tagged for removal.
Because you are building a substitute, you do not need to worry about the Output Type. However, you can still set the template, file name, file location and BOM Structure. The Style is the same as it is with derive: Single Solid No Seams, Single Solid with Seams, Multi-body Solid and Single Composite.
The Advanced Properties section provides additional options. When creating a substitute, these should be enabled:
- Fill internal voids fills (removes) all internal void shells in the resultant part.
- Remove internal parts for Inventor to evaluate the model from the 14-standard orthographic and isometric directions. Components Inventor deems hidden (from all angles) are removed.
When Link face color from source component is unchecked, Inventor sets the appearance to the default appearance of the target model.
You want to use Make for independent bodies on failed Boolean when encountering errors with the simplified model. This can help find the specific components that are causing the issues.
What Should I Use?
The Derive Assembly option simplifies the assembly using the Derived Component functionality. The Simplify option creates a simplified part in the same way as one uses the Simplify tool. In both cases, Inventor creates a new substitute part and the model state uses it.
I will use derive with assemblies for which I have not built lower-level model states. In these cases, I like working with the hierarchical view dialog. I can exclude subassemblies or the components of subassemblies. I appreciate the ability to pick the Boolean operation and select the components to exclude and the ones to convert to bounding boxes. A caveat: This was also the first option Inventor had and we tend to fall back on what we know best and what we have used the most often.
Simplify reduces model complexity with a focus on removing unnecessary details or features. With its built-in presets and the ability to create your own presets, this can be the quicker choice. Because it uses the property palette interface, it is also the easier choice to use and learn. It is also better at removing features.
How does one decide which to use? The saying goes six of one, half a dozen of the other. In most cases, it does not matter. The choice depends on specific needs but typically comes down to personal preference.
Bill of Materials and Drawings
A substitute state uses a single part to replace an assembly. If Inventor showed the BOM of the substitute, it would only be a single line. Instead, Inventor shows the Primary state’s BOM. To make sure you know this, it prompts you about the delegation.
You also will see this with migrated levels of detail. The Level of Detail feature set was replaced by Model States in Inventor 2022.
You can select any model state when creating drawing views, including substitutes. For the same reasons that substitutes improve assembly performance, they can also improve drawing performance. However, you want to use only one model state per drawing. By using more than one, you impact performance negatively because Inventor loads each state used in the drawing in the background .
Therefore, use just one model state in your drawings and use View Representations to manage component visibility in the view. You can read more about representations here.
Model States and Autodesk Vault
Autodesk Vault offers support for Model States.
You can open and place files into Inventor by selecting different states.
When looking at files (Project Explorer), Vault displays the properties of the Primary state. Use the Model State-related system properties to help identify the files with model states:
- Has Model State shows if the file has model states (more than just Primary).
- Is True Model State will be true if the part number does not vary between states.
- Is Table Driven is true when the file is an iComponent (iPart/iAssembly) or has multiple Model States.
In this example, Vault is showing the part number and description for the Primary state of the Suspension-Fork assembly. As it has multiple states, Has Model State is showing the icon and Is Table Driven is checked (true). As it has states with different part numbers, Is True Model State is false (empty).
As model states support unique iProperties, parameters and BOM, you can use states to build configurations of the assemblies. With Items, Vault creates an item for each model state with different part numbers, allowing you to manage the life cycles of these configurations. Note that this is only available with Vault Professional.
As Inventor stores the model state configurations in a singular file, the file attaches to each item.